|
*COMMAND (Functions
of midas) |
|
Brief descriptions of the Commands |
|
; Variables that make
up the Commands |
|
Description of each variable
(method of expression) {initialized value} |
* X,Y,Z axis: Basis of Global coordinates
x,y,z axis: Basis of nodal or element local coordinates
|
*VERSION |
|
Shows the version of MIDAS/Gen |
|
*UNIT (Unit
System) |
|
; FORCE, LENGTH |
|
; FORCE, LENGTH |
|
FORCE:
Loading unit used in creating MGT File {tonf}
:LENGTH
Length unit used in creating the MGT File {m} |
|
* ENDDATA (End
Data) |
|
Completion of Data input |
|
*PROJINFO (Project
Information) |
|
Basic project data |
|
PROJECT, REVISION, USER,
EMAIL, ADDRESS,
TEL, FAX, CLIENT, TITLE,
ENGINEER, EDATE
CHECK1, CDATE1, CHECK2,
CDATE2, CHECK3,
CDATE3, APPROVE, ADATE,
COMMENT |
|
PROJECT: project
name
REVISION: date
of final revision
USER:
user name
EMAIL: e-mail
address
ADDRESS: postal
address line
FAX:
fax number
CLIENT:
client name
TITLE:
sub-title of project (sub-project name)
ENGINEER:
name of engineer
EDATE:
date of program operation
CHECK1: 1st
reviewer
CDATE1 :
date of 1st review
CHECK2:
2nd reviewer
CDATE2:
date of 2nd review
CHECK3:
3nd reviewer
CDATE3:
date of 3nd review
APPROVE:
final approver
ADATE:
date of final approval
COMMENT:
notes & comments |
|
*STRUCTYPE (Structure
Type) |
|
Basic data required for Structural Analysis |
|
; iSTYP, iSMAS, GRAV,
TEMPER, bALIGNBEAM,
bALIGNSLAB |
|
iSTYP:
structural type {0}
= 0: 3-dimensional analysis
= 1: 2-dimensional analysis
(X-Zplane)
= 2: 2-dimensional analysis
(Y-Zplane)
= 3: 2-dimensional analysis
(X-Yplane)
= 4: 3-dimensional analysis
(restraint on rotational degree of
freedom about Z-direction)
iSMAS: assigns
whether to convert the model self-weight to
masses {0}
= 0: does not convert
to masses
= 1: converts to masses
& applies to X,Y,Z directions in the global
coordinate system
= 2: converts to masses
& applies to X,Y directions in the global
coordinate system
= 3: converts to masses
& applies to Z direction in the global
coordinate system
GRAV:
value of acceleration of gravity considering the applied
units {9.806 m/sec2}
TEMPER:
initial temperature required for heat stress analysis
bALIGNBEAM:
alligns the tops of girders to Floor Level
(YES/NO) {NO}
bALIGNSLAB:
alligns the top of slabs to Floor Level
(YES/NO) {NO} |
|
*GRIDLINE*(Define
Line Grid) |
|
Gridline |
|
; NAME, X, Y |
|
NAME:
name of gridline
X:
X coordinates of GCS (Global Coordinate System) Y-axis
direction and gridlines
Y:
Y coordinates of GCS (Global Coordinate System) X-axis
direction and gridlines |
|
*NODE
(Nodes) |
|
Node data |
|
; iNO, X, Y, Z |
|
iNO:
node number
X: X-coordinate
in GCS (Global Coordinate System)
Y: Y-coordinate
in GCS (Global Coordinate System)
Z: Z-coordinate
in GCS (Global Coordinate System) |
|
*ELEMENT (Elements) |
|
Element Data |
|
; iEL, TYPE, iMAT, iPRO,
iN1, iN2, ANGLE,
iSUB, EXVAL ;
Frame Element
; iEL, TYPE, iMAT, iPRO,
iN1, iN2, iN3, iN4
iSUB, iWID ;
Planar Element
; iEL, TYPE, iMAT, iPRO,
iN1, iN2, iN3, iN4,
iN5, iN6, iN7, iN8 ;
Solid Element |
|
1.Frame Element
iEL: element
number
TYPE: element
type
=TRUSS: truss
element
=BEAM: beam
element
=TENSTR:
tension-only element
=COMPTR:
compresion-only element
iMAT:
material number
iPRO:
section number
iN1: 1st
node number
iN2: 2nd
node number
ANGLE:
Beta Angle
iSUB:
Sub Type
For Truss: N/A
For Beam: N/A
For TENSTR & COMPTR
{1}
=1: TENSTR-TRUSS, COMPTR-TRUSS
=2: TENSTR-HOOK, COMPTR-GAP
=3: TENSTR-CABLE
EXVAL:
additional data related to entered elements
For Truss: N/A
For Beam: N/A
For TENSTR
=TRUSS: N/A
=HOOK: Hook Distance
=Cable: Cable Pretension
For COMPTR
=TRUSS: N/A
=GAP: Gap Diatance
= WALL: wall element
2. Planar Element
iEL: element
number
TYPE: element
type
=PLATE: plate element
=PLSTRS: plane stress
element
=PLSTRN: plane strain
element
=AXISYM: axis symmetric
element
iMAT: material
number
iPRO:
section number
iN1: 1st
node number
iN2:
2nd node numberiN
iN3: 3rd
node number
iN4: 4th
node number
iSUB: Sub
Type
For Plate {1}
=1: Thick =
2: Thin
For PLSTRS: N/A
For PLSTRN: N/A
For Axisymmetric: N/A
For Wall {1}
=1: Membrane
=2: Plate
iWID: wall (combination
of elements) ID
3.Solid Element
iEL: element
number
TYPE : element type
=SOLID: solid element
iMAT: material
number
iPRO: section
number
iN1: 1st
node number
iN2: 2nd
node number
iN3: 3rd
node number
iN4: 4th
node number
iN5: 5th
node number
iN6:
6th node number
iN7: 7th
node number
iN8: 8th
node number
4. Frame (Ref. Point)
REF: assign
ref. point
RPX: X-coordinate
of ref. point
RPZ:
Z-coordinate of ref. point |
|
*MATERIAL
(Material) |
|
Material property |
|
; iMAT, TYPE, MNAME, SPHEAT,
HEATCO, [DATA1]
; STEEL, CONC, USER
; iMAT, TYPE, MNAME, SPHEAT,
HEATCO, [DATA1],
[DATA2] ;
SRC
; [DATA1]: 1, DB, NAME
2, ELAST, POISN, THERMAL,
DEN
3, Ex, Ey, Ez, Tx, Ty,
Tz, Sxy, Sxz, Syz, Pxy, Pxz,
Pyz, DEN : Orthotropic
; [DATA2]: 1, DB, NAME
or 2, ELAST, POISN, THERMAL
DEN |
|
iMAT: material
number
TYPE: material
type
=STEEL (structural steel)
=CONC (concrete)
=SRC(steel-concrete composite)
=USER(user defined)
MNAME: material
name
SPHEAT:
specific heat
HEATCO:
thermal conductivity coefficient
[DATA 1]
DB: section
database of various national standards
NAME:
name of DB
[DATA 2]
ELAST:
modulus of elasticity
POISN: poisson’s
ratio
THERMAL:
coefficient of linear thermal expansion
DEN:
weight per unit volume
1. Orthoropic: for orthotropic material
Ex, Ey, Ez: modulii
of elasticity in the corresponding directions
Tx, Ty, Tz: coefficients
of linear thermal expansion in the
corresponding directions
Sxy, Sxz, Syz: shear
modulii of elasticity in the corresponding
directions
Pxy, Pxz, Pyz: poisson’s
ratios in the corresponding directions |
|
*MATL-COLOR |
|
Color data for materials |
|
; iMAT, W_R, W_G, W_B,
HF_R, HF_G, HF_B,
HE_R, HE_G, HE_B, bBLEND,
FACT |
|
iMAT: material
number
W_R: red
color number when displaying in Wire Frame
W_G: green
color number when displaying in Wire Frame
W_B: blue
color number when displaying in Wire Frame
HF_R:
red color number of Hidden treated surface
HF_G: green
color number of Hidden treated surface
HF_B:
blue color number of Hidden treated surface
HE_R:
red color number of the outline of Hidden treated surface
HE_G:
green color number of the outline of Hidden treated surface
HE_B:
blue color number of the outline of Hidden treated surface
bBLEND:
assigns color transparency
(YES/NO) {NO}
FACT:
factor (degree) of color transparency {0.5} |
|
*TDM-FUNC (Time Dependent
Material Function) |
|
Creep/Shrinkage function of concrete |
|
; FUNC=NAME, FTYPE, SCALE,
CTYPE, ELAST
DESC
;
line 1
; DAY1, VALUE1, DAY2,
VALUE2,? ;
from line 2 |
|
NAME:
function name that defines Creep (Shrinkage)
FTYPE: function
type
= CREEP: creep of concrete
= SHRINK: shrinkage of
concrete
SCALE: scale
factor
CTYPE: creep
function data type
= SC: Specific Creep
= CF: Creep Compliance
= CC: Creep Coefficient
ELAST:
modulus of elasticity of concrete
DESC:
brief description
DAY1: time
VALUE1:
creep /shrinkage data value |
|
*TDM-TYPE (Time Dependent Material) |
|
Time dependent material data (creep, shrink) |
|
; NAME=NAME, CODE, STR,
HU, VOL, AGE, TYPE, [ACI1],
[ACI2] ;
CODE=ACI
; NAME=NAME, CODE, STR,
HU, MSIZE, CTYPE, AGE
; CODE=CEB, KS
; NAME=NAME, CODE, N1,
PHI1, N2, PHI2
; CODE=MEM
; NAME=NAME, CODE, STR,
HU, USS, UCS, VOL, RR
MOD ;
CODE=PCA
; NAME=NAME, CODE, STR,
HU, VOL, UCS, VSR1, LAF
VSR, PST, bRCE, RR, MOD
;
CODE=COMBINED
; N
AME=NAME, CODE, STR, HTYPE,
HU, MSIZE
CTYPE, AGE ;
CODE=JAPAN
; NAME=NAME, CODE, STR,
HTYPE, HU, MSIZE
AGE ;
CODE=CHINA
; NAME=NAME, CODE, bSSF,
SSFNAME
; CODE=USER (line 1)
; CREEPFUNC1, AGE1, CREEPFUNC2,
AGE2, ...
; USER (from line 2)
; [ACI1]: CURE, SLUMP,
FAP, AIR, CC
; [ACI2]: UCC, USS |
|
1. Common Items
NAME: Time
dependent material name
CODE: DB
of time dependent material
=ACI: American Concrete
Institute
= KS: Korean Standard
= MEM: Modify Elasticity
Modulus, consider creep by
modifying the elasticity
of modulus.
= JAPAN: Japanese Standard
= CHINA: Chinese Standard
= USER: user directly
specifies material data
2. In the case of ACI
STR: 28
day compressive strength
HU: relative
humidity
VOL:
volume-surface area ratio
AGE: start
time of shrinkage after casting concrete
TYPE: ultimate
factor reflecting the properties of concrete
3. In the case of CEB, KS
MSIZE: notational
size of structure
CTYPE: type
of cement
= RS: Rapid hardening
high strength cement
= NR: Normal or rapid
hardening cement
= SL:
Slowly hardening cement
4. In the case of MEM
N1: number
of days between 0 (day) & N1 (day)
PHI1: reduction
factor for modulus of elascity
5. In the case of PCA
STR:
28 day compressive strength
HU: relative
humidity
USS: ultimate
shrinkage strain
UCS: ultimate
creep strain
VOL:
volumn-surface area ratio
RR: reinforcement
ratio of column
MOD:
modulus of elasticity of reinforcement
6. In the case of COMBINED
STR: 28
days compressive strength
HU: relative
humidity
VOL: volumn-surface
area ratio
UCS:
ultimate creep strain
VSR1: volumn-surface
area ratio
LAF:
age factor calculation
US: ultimate
shrinkage strain
VSR:
volumn-surface area ratio
PST:
state of progress of shrinkage
bRCE: whether
or not the reinforced concrete effect by PCA is
applied
RR:
reinforcement ratio of column
MOD: modulus
of elasticity of reinforcement
7. In the case of JAPAN
STR:
28 day compressive strength
HTYPE: type of curing
= CM: water-immerced curing
= RM: ambient curing
HU:
relative humidity
MSIZE :
notational size of structure
CTYPE: type
of cement
= RN: rapid hardening
Cement
= NC: normal Cement
AGE: start
time of shrinkage after casting concrete
[ACI1] or [ACI2]
CURE:
initial curing method
SLUMP:
concrete slump value
FAP:
fine aggregate ratio
AIR: air
entraintment quantity
CC:
cement quantity
UCC:
ultimate creep coefficient
USS:
ultimate shrinkage strain
8. In the case of CHINA
STR: 28
day compressive strength
HTYPE: type
of curing
= CM: water-immerced curing
= RM: ambient curing
HU: relative
humidity
MSIZE:
notational size of structure
AGE: start
time of shrinkage after casting
9. In the case of USER
bSSF:
whether or not Shrinkage Strain Function is applied
SSFNAME: shinkage
function to be applied
CREEPFUNC1:
creep function to be applied
AGE1: age
(elapsed time) at the time of load application |
|
*TDM-ELAST |
|
Time Dependent Material (Comp. Strength)
Change of Modulus of Elasticity (compressive
strength) relative to concrete maturity
(age) |
|
; NAME=NAME, TYPE, CODE,
STRENGTH, A, B
; TYPE=CODE (Korean Standard,
ACI)
; NAME=NAME, TYPE, CODE,
STRENGTH, iCTYPE
; TYPE=CODE (CEB-FIP,
Ohzagi)
; NAME=NAME, TYPE, CODE,
STRENGTH
; TYPE=CODE (Chinese Standard)
; NAME=NAME, TYPE, SCALE
; TYPE=USER (line 1)
; DAY1, VALUE1, DAY2,
VALUE2, ...
; USER (from line 2) |
|
1. Common Items
NAME:
function name that defines the change of Modulus of
Elasticity (compressive
strength) relative to concrete maturity
TYPE:
input method for the change of Modulus of Elasticity
(compressive strength)
=CODE: select concrete
specs defined in the code
= USER: user directly
specifies the change of Modulus
Elasticity
CODE: selected
code name
=ACI
= CEB-FIP
= Ohzagi
= Chinese Standard
= Korean Standard
2.In the case of KS,
STRENGTH: concrete
compressive strength relative to curing
time
=KS: concrete compressive
strength at 91 days
=ACI: concrete compressive
strength at 28 days
A,B: factors for compressive
strength of concrete
3.In the case of CEB-FIP, Ohzagi
iCTYPE: different
types of cement modulus
= 1: Rapid hardening high
strength cement
= 2: Normal or rapid hardening
cement
= 3: Slowly hardening
cement
= 4: In cases of using
flyash
4. In the case of USER
SCALE:
scale factor
DAY1: time
VALUE1: data
value of elastic modulus |
|
*TDM-LINK (Time
Dependent Material Link) |
|
Assigns time dependent properties of materials
to the
initially entered normal material data |
|
; iMAT, TDM-TYPE1 (CREEP/SHRINKAGE),
TDM-TYPE2 (ELASTICITY) |
|
iMAT:
material number, which assigns time dependent properties
TDM-TYPE1 (CREEP/SHRINKAGE):
selects a material
property, which has been
defined in the Time Dependent Material
(Creep/Shrinkage)
TDM-TYPE2 (ELASTICITY) :
selects a material, which
has been defined in the Time Dependent
Material (Elasticity) |
|
*ELEM-DEPMATL (Change
Element Dependent Material Property) |
|
Modifies Notational size (h), which is
applied in the
automatic calculation of time dependent
property |
|
; ELEM_LIST, H |
|
ELEM_LIST:
list of element numbers to be changed
H: geometric
shape factor (h, Notational Size of Member |
|
*SECTION (Section) |
|
Section data of truss or beam elements |
|
; iSEC, TYPE, SNAME, OFFSET,
SHAPE, [DATA]
{, CCSHAPE} ;
DB/USER
; iSEC, TYPE, SNAME, OFFSET,
SHAPE, BLT, D1, D2, D3
D4, D5, D6 ;
1st line - VALUE
; AREA, ASy, ASz, Ixx,
Iyy, Izz ;
2nd line
; CyP, CyM, CzP, CzM,
QyB, QzB, PERI_OUT, PERI_IN,
Cy, Cz ;
3rd line
; iSEC, TYPE, SNAME, OFFSET,
SHAPE,
iREPLACE, ELAST, DEN,
POIS, POIC ;
1st line - SRC
; D1, D2, [DATA] ;
2nd line
; iSEC, TYPE, SNAME, OFFSET,
SHAPE, 1, DB, NAME1
NAME2, D1, D2 ;
COMBINED
; iSEC, TYPE, SNAME, OFFSET,
SHAPE, 2, D11, D12,
D13, D14, D15, D21, D22,
D23, D24]
; iSEC, TYPE, SNAME, OFFSET,
SHAPE, iyVAR, izVAR
STYPE ;
1st line - TAPERED
; DB,NAME1,NAME2
;
2nd line(STYPE=DB)
; [DIM1],
[DIM2] ;
2nd line (STYPE=USER)
; D11,
D12, D13, D14, D15, D16
; 2nd line (STYPE=VALUE)
; AREA1,
ASy1, ASz1, Ixx1, Iyy1, Izz1
; 3rd line (STYPE=VALUE)
; CyP1,
CyM1, CzP1, CzM1, QyB1, QzB1, PERI_OUT1,
PERI_IN1, Cy1, Cz1 ;
4th line (STYPE=VALUE)
; D21,
D22, D23, D24, D25, D26
; 5th line (STYPE=VALUE)
; AREA2,
ASy2, ASz2, Ixx2, Iyy2, Izz2
; 6th line (STYPE=VALUE)
; CyP2,
CyM2, CzP2, CzM2, QyB2, QzB2, PERI_OUT2
PERI_IN2, Cy2, Cz2 ;
7th line (STYPE=VALUE)
[DATA]: 1, DB, NAME or
2, D1, D2, D3, D4, D5, D6
; [DIM1], [DIM2] : D1,
D2, D3, D4, D5, D6 |
|
1. Common Items
iSEC: section
number
TYPE: type
of section property
= DBUSER: selected from
DB or standard section
= VALUE: directly specified
section property data
= SRC: section property
of SRC member
=COMBINED: section property
of combined sections
SNAME: section
name
SHAPE:
shape symbol of section (refer to Table 1 below)
2. DB/USER
CCSHAPE:
cold formed section data
3.
In the case of VALUE
BLT:
classifies builtup methods of members
D1~D6:
dimensions of section
AREA~Cz:
section stiffness data
*refer
to on-line manual
4. In the case of SRC
iREPLACE: reference
material used for calculating the
stiffness of composite
sections
=1: Steel =2:
Concrete
ELAST:
ratio of modulus of elasticity of steel to concrete
DEN:
ratio of steel density to concrete
POIS:
poisson’s ratio for steel
POIC:
poisson’s ratio for concrete
D1, D2:
dimensions of a concrete section
7. COMBINED
1: selecting
a section from DB
DB: DB
of standard sections
NAME1, NAME2: names
of two section types, which make
up the combined section
D1: 1st
dimension of a section
D2:
2nd dimension of a section
2: when
ispecifying the main dimensions of standardized sections
(USER)
D11:
1st dimension of a section
D12: 2nd
dimension of a section
D13:
3rd dimension of a section
D14:
4th dimension of a section
D15:
5th dimension of a section
D16: 6th
dimension of a section
D21:
7th dimension of a section
D22:
8th dimension of a section
D23:
9th dimension of a section
D24:
10th dimension of a section
D25: 11th
dimension of a section
D26:
12th dimension of a section
8.
TAPERED
iyVAR:
method of calculating moment of inertia about the y-axis
of the element local coordinate
system {1}
= 1: 1st (Linear)
= 3: 3rd (Cubic)
izVAR:
method of calculating moment of inertia about the z-axis
of the element local coordinate
system {1}
= 1: 1st (Linear)
= 2: 2nd (Parabolic)
= 3: 3rd (Cubic)
STYPE:
assigns the section type of a tapered section member to
be used |
|
L |
Angle |
C |
Channel |
I |
I-Section |
|
T |
T-Section |
B |
Box |
P |
Pipe |
|
2L |
Double Angle |
2C |
Double Channel |
SB |
Solid Rectangle |
|
SR |
Solid Round |
CC |
Cold Formed Channel |
|
|
Table 1. Shape symbols of input sections (SNAME)
|
*SECT-COLOR |
|
Color data of sections |
|
; iSEC, W_R, W_G, W_B,
HF_R, HF_G, HF_B, HE_R, HE_G,
HE_B, bBLEND, FACT |
|
iSEC:
section number
W_R: red
color number when displaying in Wire Frame
W_G: green
color number when displaying in Wire Frame
W_B: blue
color number when displaying in Wire Frame
HF_R: red
color number of Hidden treated surface
HF_G:
green color number of Hidden treated surface
HF_B:
blue color number of Hidden treated surface
HE_R: red
color number of the outline of Hidden treated surface
HE_G:
green color number of the outline of Hidden treated surface
HE_B: blue
color number of the outline of Hidden treated surface
bBLEND: assigns
color transparency
(YES/NO) {NO}
FACT: factor
(degree) of color transparency {0.5} |
|
*SECT-SCALE (Section
Stiffness Scale Factors) |
|
Stiffness scale factors applicable to the
section
properties of line elements |
|
; iSEC, AREA_SF, ASY_SF,
ASZ_SF, IXX_SF, IYY_SF,
IZZ_SF, WGT_SF |
|
iSEC: section
subject to scale factors
AREA_SF:
scale factor for section area
ASY_SF: scale
factor for effective section area, which resists the y-
axis direction shear force
in the element local coordinate system
ASZ_SF: scale
factor for effective section area, which resists the z-
axis direction shear force
in the element local coordinate system
IXX_SF:
scale factor for torsional moment of inertiaa
IYY_SF: scale
factor for moment of inertia about the y-axis in the
element local coordinate
system
IZZ_SF:
scale factor for moment of inertia about the z-axis in the
element local coordinate
system
WGT_SF: scale
factor for section weight |
|
*TS-GROUP (Tapered
Section Group) |
|
Grouping Tapered Section members |
|
; NAME, ELEM_LIST, ZVAR,
ZEXP, ZFROM, ZDIST,
YVAR, YEXP, YFROM, YDIST |
|
NAME: group
name of tapered section
ELEM_LIST: element
numbers included in the tapered section group
ZVAR:
defines the change of section shape in the z-axis direction of the element
local coordinate system
= Linear: linear change
following a straight line
= Quadratic: Quadratic
change following a 2 dimensional curve
ZEXP:
assigns the exponent (1~2) of the function defining the shape
change of section
ZFROM:
origin point for defining the mirror plane
ZDIST: distance
from the origin point to the mirror plane in the x-
direction
of the element local coordinate system
YVAR: defines
the change of section shape in the y-direction of
the element local coordinate
system |
|
*THICKNESS (Thickness) |
|
Thickness data for planar elements |
|
; iTHK, TYPE, bSAME, THIK-IN,
THIK-OUT
; TYPE=VALUE
; iTHK, TYPE, SUBTYPE,
RPOS, WEIGHT
; TYPE=STIFFENED, SUBTYPE=VALUE
; SHAPE,
THIK-IN, THIK-OUT, HU, HL
; for yz section
; SHAPE,
THIK-IN, THIK-OUT, HU, HL
; for xz section
; iTHK, TYPE, SUBTYPE,
RPOS, PLATETHIK
; TYPE=STIFFENED, SUBTYPE=USER
; bRIB
{, SHAPE, DIST, SIZE1, SIZE2, ..., SIZE6}
;
for yz section
; bRIB
{, SHAPE, DIST, SIZE2, SIZE2, ..., SIZE6}
; for xz section
; iTHK, TYPE, SUBTYPE,
RPOS, PLATETHIK, DBNAME
; TYPE=STIFFENED, SUBTYPE=DB
; bRIB
{, SHAPE, DIST, SNAME}
; for yz section
; bRIB
{, SHAPE, DIST, SNAME}
; for xz section |
|
1. Common Items
iTHK: thickness
ID number
TYPE: method
of defining thickness data
=VALUE
2.
=STIFFENED
2. If Type is ‘Value’
bSAME: applies
the same thickness to both in-plane and out-of-
plane (bending) thicknesses
(YES/NO) {YES}
THIK-IN: thickness
applied to calculate the in-plane stiffness
THIK-OUT: thickness
applied to calculate the out-of-plane stiffness
3. If Type is ‘Stiiffered’ and
Subtype is‘Value’
SUBTYPE:
method of defining the thickness data
=
VALUE
=
USER
=
DB
RPOS: rib
position
= LOWER
= UPPER
WEIGHT: equivalent
thickness data for weight calculation
SHAPE: selects
the rib section
THIK-IN: thickness
applied to calculate the in-plane stiffness
THIK-OUT: thickness
applied to calculate the out-of-plane stiffness
4. If Type is ‘Stiiffered’ and
Subtype is ‘User’
SUBTYPE, RPOS:
refer to #3
PLATETHIK:
thickness data of plate element
bRIB:
selects whether or not ribs exist
SHAPE: assigns
the section shape of the rib
DIST: distance
(spacing) between the ribs
SIZE1~ SIZE6: section
size of the rib
5. If Type is ‘Stiiffered’ and
Subtype is ‘DB’
SUBTYPE, RPOS: refer
to #3
PLATETHIK: thickness data of plate element
DBNAME:
name of DB
bRIB: selects
whether or not ribs exist
SHAPE:
assigns the section shape of the rib
DIST: distance
(spacing) between the ribs
SNAME: section
name |
|
*THIK-COLOR |
|
Color data for individual thickness numbers |
|
; iTHK, W_R, W_G, W_B,
HF_R, HF_G, HF_B, HE_R, HE_G
HE_B, bBLEND, FACT |
|
iTHK: thickness
ID number
W_R:
red color number when displaying in Wire Frame
W_G:
green color number when displaying in Wire Frame
W_B:
blue color number when displaying in Wire Frame
HF_R: red
color number of Hidden treated surface
HF_G: green
color number of Hidden treated surface
HF_B:
blue color number of Hidden treated surface
HE_R: red
color number of the outline of Hidden treated surface
HE_G:
green color number of the outline of Hidden treated surface
bBLEND: assigns
color transparency
(YES/NO) {NO}
FACT: factor
(degree) of color transparency {0.5} |
|
*THIK-COLOR |
|
Color data for individual thickness numbers |
|
; iTHK, W_R, W_G, W_B,
HF_R, HF_G, HF_B, HE_R, HE_G,
HE_B,
bBLEND, FACT |
|
iTHK: thickness
ID number
W_R: red
color number when displaying in Wire Frame
W_G: green
color number when displaying in Wire Frame
W_B: blue
color number when displaying in Wire Frame
HF_R: red
color number of Hidden treated surface
HF_G:green
color number of Hidden treated surface
HF_B: blue
color number of Hidden treated surface
HE_R: red
color number of the outline of Hidden treated surface
HE_G: green
color number of the outline of Hidden treated surface
HE_B:
blue color number of the outline of Hidden treated surface
bBLEND: assigns
color transparency
(YES/NO) {NO}
FACT: factor
(degree) of color transparency {0.5} |
|
*TDN-PROPERTY (Tendon
Property) |
|
Tendon property and assigning the methods
of
prestress application |
|
; NAME, TYPE, MATL, AREA,
DIA, RC, FF, WF, US, YS,
LT,
ASB, ASE, |
|
NAME: name of tendon to
be defined
TYPE: type of tendon classified
by the location of the tendon
relative to the element
section
= Internal: located within
the section
= External: located outside
of the section
AREA: total area of the
tendon
DIA: diameter of the duct
RC: C, Relaxation Coefficient
FF: Friction Factor
WF: Wobble Factor
US: Ultimate Strength
YS: Yield Strength
LT: method of tensioning
= Pretension
= Post-tension
ASB: magnitude of slip
at the tensioning anchorage
ASE: magnitude of slip
at the end anchorage |
|
*TDN-PROFILE
(Tendon Profile) |
|
Placing arrangement and defining the shape
of
tendon
relative to the element section |
|
; NAME=NAME, TDN-PROPERTY,
ELEM_LIST, BEGIN
END, CURVE ;
line 1;
; SHAPE,
IP_X, IP_Y, IP_Z, AXIS, VX, VY
;
line 2 (SHAPE=STRAIGHT)
; SHAPE, IP_X, IP_Y, IP_Z,
RC_X, RC_Y, OFFSET
;
line 2 (SHAPE=CURVE)
; XAR_ANGLE,
bPROJECTION, GR_AXIS,
GR_ANGLE
;
line 3
; X1,
Y1, Z1, bFIX1, RY1, RZ1, RADIUSI
; from line 4
; ...
; Xn,
Yn, Zn, bFIXn, RYn, RZn, RADIUSn |
|
NAME:
tendon name
TDN-PROPERTY: assigns
tendon properties
ELEM_LIST:
element numbers for tendon assignment
BEGIN:
straight distance of the tendon at the beginning
END:
straight distance of the tendon at the end
CURVE:
curved shape of tendon
= SPLINE
= ROUND
1. In the case of STRAIGHT
SHAPE:
shape of the imaginary axis, which is referenced for
placing the straight tendon
IP_X: X-coordinate
of Profile Insertion Point
IP_Y:
Y-coordinate of Profile Insertion Point
IP_Z: Z-coordinate
of Profile Insertion Point
AXIS: defines
the x-axis direction in the tendon coordinate
system if the tendon is
placed straight
VX: x-axis
is parallel with the X-axis of the global coordinate system
VY: x-axis
is parallel with the Y-axis of the global coordinate system
2. In the case of CURVE
SHAPE: shape
of the imaginary axis, which is referenced for placing
the curved tendon
IP_X: X-coordinate
of Profile Insertion Point
IP_Y: Y-coordinate
of Profile Insertion Point
IP_Z: Z-coordinate
of Profile Insertion Point
RC_X:
center x-coordinate of the reference circle in the global
coordinate system if tendon
is placed curvilinearly
RC_Y: center
y-coordinate of the reference circle in the
coordinate system if tendon
is placed curvilinearly
OFFSET:
places the tendon in the location projected in the
direction of the radius
of the circle
XAR_ANGLE: rotation
angle about the x-axis in the tendon
coordinate system (convenient
when placing sloped web tendons)
bPROJECTION: defines
whether or not to place the tendon at
the
location projected onto the plane after rotation (YES/NO)
GR_AXIS: reference
axis about which is rotated
GR_ANGLE: rotation
angle about the Y or Z axis in the global coordinate system
X1: X-coordinate
of the point through which the tendon passes
based on the tendon coordinate
system
Y1: Y-coordinate
of the point through which the tendon passes
based on the tendon coordinate
system
Z1: Z-coordinate
of the point through which the tendon passes
based on the tendon coordinate
system
bFIX1: whether
or not to fix the tangent angle of the tendon
(YES/NO)
RY1: tangent
angle relative to the x-axis in the
x-z
plane in the tendon coordinate system when the tangent angle is fixed
RZ1: tangent
angle relative to the x-axis in the
x-y plane in the tendon
coordinate system when the tangent angle is fixed
RADIUS: radius
of the circle in tangent with the straight line oftendon |
|
*CONSTRAINT(Supports) |
|
Conditions restraining the nodal degrees
of freedom |
|
; NODE_LIST, CONST (Dx,
Dy, Dz, Rx, Ry, Rz), GROUP |
|
NODE_LIST:
node number
CONST (Dx, Dy, Dz, Rx, Ry, Rz): components
of degrees of
freedom identified in
6 Digit
CodeGROUP:
Boundary Group Name |
|
*SPRING (Point Spring Supports) |
|
Elastic support conditions assigned to
nodes |
|
; NODE_LIST, SDx, SDy,
SDz, SRx, SRy, SRz, GROUP |
|
NODE_LIST: node
number
SDx: spring
constant in the x-axis direction [force/length]
SDy: spring
constant in the y-axis direction [force/length]
SDz: spring
constant in the z-axis direction [force/length]
SRx: rotational
spring constant about the x-axis direction
[moment/angle]
SRy: rotational
spring constant about the y-axis direction
[moment/angle]
SRz:
rotational spring constant about the z-axis direction
[moment/angle]
GROUP: Boundary
Group Name |
|
*GSPRTYPE (Define General Spring Supports) |
|
Stiffness of a general support spring |
|
; NAME, SDx1, SDy1, SDy2,
SDz1, SDz2, SDz3, ...,
SRz1,
..., SRz6 |
|
NAME: name
of spring stiffness
SDx1: spring
stiffness in the global or local x-axis direction
SDy1, SDy2: spring
stiffness interrelated in the global or local x-
and y-axis directions
SDz1, SDz2, SDz3: spring
stiffness interrelated in the global or
local x-, y- and z-axis
directions
SRz1, ? SRz6: rotational
spring stiffness interrelated in
the global or local x-,
y- and z-axis directions |
|
*GSPRING (General Spring Supports) |
|
Conditions of a general spring support
assigned to nodes |
|
; NODE_LIST, TYPE-NAME,
GROUP |
|
NODE_LIST:
node number
TYPE-NAME:
name of General Spring Type
GROUP: Boundary
Group Name |
|
*ELASTICLINK |
|
Elastic link elements connecting two nodes |
|
; iNODE1, iNODE2, Link,
ANGLE, SDx, SDy, SDz, SRx, SRy,
SRz, DRy, DRz, GROUP ;
GEN
; iNODE1, iNODE2, Link,
ANGLE, bSHEAR, DRy, DRz,
GROUP ;
RIGID
; iNODE1, iNODE2, Link,
ANGLE, SDx, bSHEAR, DRy, DRz
GROUP ;
TENS, COMP |
|
iNODE1: 1st
node number of an elastic link
iNODE2:
2nd node number of an elastic link
Link: assigns
the type of the elastic link element {GEN}
= GEN: directy uses the
stiffness values that the user specifies
= RIGID: ridgid link stiffness
automatically assigned by the program
= TENS: uses as a tension-only
element
= COMP: uses as a compression-only
element
ANGLE: Beta
Angle of the elastic link element
SDx:
spring constant in the x-axis direction [force/length]
SDy:
spring constant in the y-axis direction [force/length]
SDz:
spring constant in the z-axis direction [force/length]
SRx:
rotational spring constant about the x-axis direction
][moment/angle]
SRy: rotational spring constant about the y-axis
direction
[moment/angle]
SRz:
rotational spring constant about the z-axis direction
[moment/angle]
bSHEAR: whether
or not to assign the location of shear spring
DRy,
DRz: location of shear spring in the ratio of element length
GROUP: Boundary
Group Name |
|
*NL-PROP (Nonlinear
Link Property) |
|
Joint conditions of beam ends |
|
; NAME, TYPE, TW, bSSL,
DY, DZ, DESC
; bLDX, DX, bNDX, [NL_PROP]
; bLDY, DY, bNDY, [NL_PROP]
; bLDZ, DZ, bNDZ, [NL_PROP]
; bLRX, RX, bNRX, [NL_PROP]
; bLRY, RY, bNRY, [NL_PROP]
; bLRZ, RZ, bNRZ, [NL_PROP]
; [NL_PROP]: DSTIFF, DAMP,
DEXP, bRIGDBR, BSTIFF,
EFFDAMP ;
Visco-elastic Damper Type
; [NL_PROP]: STIFF, OPEN,
EFFDAMP
;
Gap Type or Hook Type
; [NL_PROP]: STIFF, YSTR,
PYS_RATIO, YEXP, PA
EFFDAMP ;
Hysteretic System Type
; [NL_PROP]: STIFF, YSTR,
PYS_RATIO, PA, PB,
EFFDAMP ;
Lead Rubber Bearing Type
; [NL_PROP]: STIFF, FCS,
FCF, RP, RADIUS, PA, PB,
EFFDAMP ;
Friction Pendulum System Type |
|
1. Common Items
NAME:
Property name of nonlinear link
TYPE: Type
of nonlinear link
=
VD: Viscoelastic Damper
=
GAP: Gap
=
HOOK: Hook
=
HS: Hysteretic System
=
LRBI: Lead Rubber Bearing Isolator
=
FPSI: Friction Pendulum System Isolator
TW
bSSL
DY
DZ
DESC |
|
*NL-LINK (Nonlinear
Link) |
|
Joint conditions of beam ends |
|
; iNODE1, iNODE2, PROP,
ANGLE, GROUP |
|
iNODE1
iNODE2
PROP
ANGLE
GROUP |
|
*FRAME-RLS (Beam
End Release) |
|
Joining conditions of bean ends |
|
; ELEM_LIST, FLAG-i, Fxi,
Fyi, Fzi, Mxi, Myi, Mzi
;
1st Line
; FLAG-j,
Fxj, Fyj, Fzj, Mxj, Myj, Mzj, GROUP
;
2nd Line |
|
1st Line
ELEM_LIST: element
number
FLAG-i: i-node
of a beam element
Fxi:
release axial force of the i-node
Fyi: release
y-direction shear force at the i-node in the element local
coordinate system
Fzi: release
z-direction shear force at the i-node in the element local
coordinate system
Mxi:
release torsional moment at the i-node
Myi:
release moment about y-direction at the i-end in the element local
coordinate system
Mzi: release
moment about z-direction at the i-end in the element local
coordinate
system
2nd Line
FLAG-j:
j-node of a beam element
Fxj:
release axial force of the j-node
Fyj: release
y-direction shear force at the j-node in the element local
coordinate system
Fzj: release
z-direction shear force at the j-node in the element local
coordinate system
Mxj: release
torsional moment at the j-node
Myj: release
moment about y-direction at the j-end in the element local
coordinate system
Mzj: release
moment about z-direction at the j-end in the element local
coordinate system
Note: Partial Fixity may
be entered as required |
|
*OFFSET (Beam
End Offsets) |
|
Rigid end offset or eccentricity at the
beam ends |
|
; ELEM_LIST, TYPE, RGDXi,
RGDYi, RGDZi, RGDXj
RGDYj, RGDZj, GROUP ;
TYPE=GLOBAL
; ELEM_LIST, TYPE, RGDi,
RGDj, GROUP
;
TYPE=ELEMENT |
|
ELEM_LIST: element
number
TYPE: type
of coordinate system
= GLOBAL: offset distances
in vectors in the global coordinate
system with respect to
the distances and directions from the node to the Offset
= ELEMENT: offset distance
relative to the x-direction of the
element local coordinate
system
In the case of GLOBAL
RGDXi:
offset distance in vector in the global X-direction at the node
RGDYi: offset
distance in vector in the global Y-direction at the i-node
RGDZi: offset
distance in vector in the global Z-direction at the i-node
RGDXj: offset
distance in vector in the global X-direction at the j-node
RGDYj: offset
distance in vector in the global Y-direction at the j-node
RGDZj:
offset distance in vector in the global Z-direction at the j-node
GROUP:
Boundary Group Name
In the case of ELEMENT
RGDi: offset
distance from the i-node in the (+) x-direction of the
element local coordinate
system
RGDj: offset
distance from the j-node in the
(-) x-direction of the
element local coordinate system
GROUP: Boundary
Group Name |
|
*PLATE-RLS (Plate
End Release) |
|
Node connecting condition (Hinge, Fixed
Joint) and
Partial Fixity in a plate element |
|
; ELEM_LIST, N1, N2, N3,
N4, GROUP |
|
ELEM_LIST: element number
N1:
Fx (Fy):
releases axial stiffness in the x (y) axis direction in the
element local coordinate
system
Fz: releases shear stiffness
in the z-direction in the element local
coordinate system
Mx: releases bending stiffness
about the x-axis in the
element local
coordinate system
My: releases bendding
stiffness about the y-axis in the
element local coordinate
system
N2, N3, N4: same
as N1
GROUP:
Boundary Group Name
* Can assign Partial Fixity
if required |
|
*RIGIDLINK
(Rigid Link) |
|
Link conditions of master and slave nodes |
|
; M-NODE, DOF, S-NODE
LIST, GROUP |
|
M-NODE: Master
Node number
DOF:
signal for specifying components of constrained degrees of freedom
(composed of a 6 Digit
Code using "1" or "0")
S-NODE LIST: list
of Slave Node numbers
GROUP: Boundary
Group Name |
|
*PANEL-ZONE |
|
Offset distance due to Panel Zone |
|
; bCALC, FACTOR, iPOSITION |
|
bCALC:
whether to automatically consider rigid end offset
(YES/NO) {YES}
FACTOR:
correction factor for rigid end offst
iPOSITION: output
location of member forces |
|
*LOCALAXIS (Node
Local Axis) |
|
Used to input boundary conditions by defining
a
nodal coordinate system at a specific node
or produce
reaction output in the nodal corrdinate
system |
|
; NODE_LIST, iMETHOD,
ANGLE-x, ANGLE-y, ANGLE-z
;
iMETHOD=1
; NODE_LIST, iMETHOD,
P0X, P0Y, P0Z, P1X, P1Y, P1Z
P2X, P2Y, P2Z ;
iMETHOD=2
; NODE_LIST, iMETHOD,
V1X, V1Y, V1Z, V2X, V2Y, V2Z
;
iMETHOD=3 |
|
NODE_LIST: node
number
iMETHOD: input
method of nodal coordinate system {1}
1 = Angle: defines the
nodal coordinate system by specifying 3rotation angles
2 = 3 Points: defines
the nodal coordinate system by specifying 3node coordinates
3 = Vector: defines the
nodal coordinate system by specifying 2vectors
1. In the case of Angle
ANGLE-X: rotational
angle about the X-axis of the GCS
ANGLE-y:
rotational angle about y’-axis rotated about the X-axis
ANGLE-z:
rotational angle about z’’-axis rotated about X and y’
axes
2. IN the case of 3 Point
P0X, P0Y, P0Z:
coordinates of origin in a nodal coordinate system
P1X, P1Y, P1Z:
coordinates of a specific point on the x-axis in NCS
P2X, P2Y, P2Z: coordinates
of a specific point moved
parrallel with the y-axis
from P1 in NCS
3. In the case of Vector
V1X, V1Y, V1Z:
x-axis direction vector from the origin of NCS
V2X, V2Y, V2Z: vector
from the origin of NCS of a point moved
by a specific distance
parrallel with the y-axis of NCS from the end point of V1 |
|
*STORY-DGROUP (Story
Diaphgram Group for Construction Stage) |
|
Assign the Strory Diaphragm information
defined automatically
by the Story function to boundary condition
group |
|
; STORY, GROUP |
|
STORY: story
name
GROUP:
Boundary Group Name |
|
*STLDCASE (Static
Load Cases) |
|
; LCNAME, LCTYPE, DESC |
|
LCNAME: name of unit load case
LCTYPE:
type of unit load case
USER = User Defined Load
D = Dead Load
L = Live Load
LR=Roof Live Load
W = Wind Load on Structure
E = Earthquake
S = Snow Load
R = Rain Load
IP = Ice Pressure
EP = Earth Pressure
WP = Ground Water Pressure
FP = Fluid Pressure
SF = Stream Flow Pressure
B = Buoyancy
CR = Creep
SH = Shrinkage
T = Temperature
PS = Prestress
CS = Construction Stage
Load
ER = Erection Load
IL = Live Load Impact
BK = Longitudinal Force
from Live Load
WL = Wind Load on Live
Load
CF = Centrifugal Force
CO = Collision Load
TPG = Rib Shortening
DESC:
description of load case |
|
*BLDG-CTRL (Building
Control Data) |
|
Nodal mass data assigned to nodes |
|
; bBASE, bMASS, bCENTER,
USE
;
Line 1
; LCNAME1, FACT1, LCNAME2,
FACT2,?/p>
YES,
20, YES, YES, LOAD
1,
1 |
|
bBASE: whether
or not to apply the height of ground surface base
LEVEL: height
of ground surface base
bMASS: whether
or not to include the mass below the base for
eigenvalue analysis
bCENTER:
whether or not to calculate the center of floor
USE:
selects the method of calculating the floor center
= MASS: calculates the
floor center using the distribution of mass
= LAOD: calculates the
floor center using static (long term) loads
If " LOAD" is selected for
USE
LCNAME1: load case
FACT1: scale factor |
|
*STORY
(Story) |
|
Story data (Defined by Z-coordinate) |
|
; NAME, LEVEL, bFLDIAP,
WINDWX, WINDWY,
WINDCX, WINDCY, ECCX,
ECCY |
|
NAME: story
name
LEVEL: global
Z-direction coordinate
bFLDIAP: whether
or not to apply the Diaphragm function to the
corresponding story (YES/NO)
WINDWX: effective
width in the X-direction subjected to Y-direction wind load
WINDWY:
effective width in the Y-direction subjected to Y-direction wind load
WINDCX: X-direction
coordinate of the point of wind load application
WINDCY: Y-direction
coordinate of the point of wind load application
ECCX: X-directional
eccentricity to calculate torsional moment due to the
story seismic load in
the Y-direction
ECCY: Y
-directional eccentricity to calculate torsional moment due to the
story seismic load in
the X-direction |
|
*NODALMASS (Nodal
Masses) |
|
Nodal mass data assigned to nodes |
|
; NODE_LIST, mX, mY, mZ,
rmX, rmY, rmZ |
|
NODE_LIST: node
numbers
mX: concentrated
mass in the X-direction in the GCS
mY: concentrated
mass in the Y-direction in the GCS
mZ: concentrated
mass in the Z-direction in the GCS r
mX: rotaional
concentrated mass about the X-direction in GCS
rmY: rotaional
concentrated mass about the Y-direction in GCS
rmZ: rotaional
concentrated mass about the Z-direction in GCS |
|
*DIAP-MASS (Floor
Diaphragm Masses) |
|
Floor mass data assigned to a specific
story in a building structure |
|
; 1, SSTORY, ESTORY, MP,
MA, XC, YC
;
point
; 2, SSTORY, ESTORY, ML,
D1, XC, YC
;
line
; 3, SSTORY, ESTORY, MA,
X1, Y1, X2, Y2, X3, Y3
;
triangle
; 4, SSTORY, ESTORY, MA,
XC, YC, D1, D2
;
rectangle
; 5, SSTORY, ESTORY, ML,
XC, YC, D1, D2, D3
;
circular arc;
6, SSTORY, ESTORY, MA,
XC, YC, D1, D2, D3, D4
;
circular area |
|
SSTORY: story
number for the starting story
ESTORY: story
number for the ending story
A. In the case of entering data as Point
Mass
MP: point
mass component in the lateral directions [Mass]
MA: rotational
mass moment of inertia about the Z-direction in GCS at the point mass
XC, YC: coordinates
of the center of the point mass in GCS
B. In the case of entering data as Line
Mass
ML: Mass
per unit length (Mass/Length)
D1: length
of the line mass
XC, YC: coordinates
of the center of the line mass in GCS
C. In the case of entering data as Triangular
Area Mass
MA:
Mass per unit area (Mass/Area)
X1, Y1:
coordinates of a corner of the triangular area
X2, Y2:
coordinates of the second corner of the triangular area
X3, Y3: coordinates
of the third corner of the triangular area
D. In the case of entering data as Rectangular
Area Mass
MA:
Mass per unit area (Mass/Area)
XC, YC: coordinates
of the center of the rectangular area in GCS
D1: length
of a side of the rectangle
D2: length
of the side of the rectangle perpendicular to D1
E. In the case of entering data as Circular
Arc Mass
ML: Mass
per unit length (Mass/Length)
XC, YC: coordinates
of the center of the circular arc in GCS
D1: angle
of the circular arc (Degree)
D2: radius
of the circular arc
D3:
angle of inclination formed by the center of the mass of the circular
arc relative to GCS X-axis
(Degree)
F. In the case of entering data as Circular
Area (fan-shaped) Mass
MA: Mass
per unit area (Mass/Area)
XC, YC: coordinates
of the center of the circle encompassing the fan-
shaped circular area in
GCS
D1: the
inner angle of the circular fan-shaped area (Degree)
D2:
radius of the fan-shaped area
D3:
width of the fan-shaped area in the radial direction
(D2=D3 if it is a full
fan)
D4:
angle of inclination formed by the center of the mass of the fan-
shaped circular area relative
to GCS X-axis (Degree) |
|
*LOADTOMASS (Loads
to Masses) |
|
Conversion of vertical loads into concentrated
mass data |
|
; *LOADTOMASS, DIR, bNODAL,
bBEAM, bFLOOR,
bPRES, GRAV
; LCNAME1, FACTOR1, LCNAME2,
FACTOR2, ...
;
from line 1 |
|
DIR: assigns
the directions in which the converted mass will be considered {XY}
bNODAL: option
to convert nodal loads (YES/NO) {YES}
bBEAM:
option to convert beam loads (YES/NO) {YES}
bFLOOR:
option to convert floor loads (YES/NO) {YES}
bPRES:
option to convert pressure loads (YES/NO) {YES}
GRAV: gravitational
acceleration {9.806 m/sec2}
LCNAME1: selects
the Load Case, which will be converted
FACTOR1: scale
factor to be applied when loads are converted into mass {1} |
|
*NAMEDPLANE
(Named Plane) |
|
Assignment of a name to a plane |
|
; NAME, TYPE, TOL, X1,
Y1, Z1, X2, Y2, Z2, X3, Y3, Z3
;NAME, TYPE, TOL, COORD |
|
NAME: plane
name
TYPE: selects
the method of assigning the plane {1}
= 1 : 3-Point
= 2 : X-Y plane
= 3 : X-Z plane
= 4 : Y-Z plane
TOL:
tolerance within which a plane is selected as the assigned plane {0.001
m}
X1, Y1, Z1:
coordinates of the 1st point on the plane in GCS
X2, Y2, Z2: coordinates
of the 2 nd point on the plane in GCS
X3, Y3, Z3: coordinates
of the 3rd point on the plane in GCS
COORD:
X, Y or Z coordinate in GCS for TYPE 2, 3 & 4 |
|
*NAMEDUCS (Named
UCS) |
|
Appllication of saved User Coordinate System
previously assigned |
|
; NAME, OX, OY, OZ, VXX,
VXY, VXZ, VYX, VYY, VYZ |
|
NAME: name
of the saved UCS
OX: X-coordinate
in GCS defining the origin of the selected UCS
OY: Y-coordinate
in GCS defining the origin of the selected UCS
OZ: Z-coordinate
in GCS defining the origin of the selected UCS
VXX: X-coordinate
in GCS for the vector defining the x-axis
direction of the selected
UCS
VXY: Y-coordinate
in GCS for the vector defining the x-axis
direction of the selected
UCS
VXZ: Z-coordinate
in GCS for the vector defining the x-axis
direction of the selected
UCS
VYX: X-coordinate
in GCS for the vector defining the y-axis
direction of the selected
UCS
VYY: Y-coordinate
in GCS for the vector defining the y-axis
direction of the selected
UCS
VYZ: Z-coordinate
in GCS for the vector defining the y-axis
direction
of the selected UCS |
|
*GROUP (Group) |
|
Grouping desired entities by assigning
a specific group name |
|
; NAME, NODE_LIST, ELEM_LIST |
|
NAME: Group
name
NODE_LIST: selected
node numbers
ELEM_LIST: selected
element numbers |
|
*BNDR-GROUP (Boundary
Group) |
|
Grouping nodes or elements constrained
with
boundary conditions by assigning a specific
boundary
group name |
|
; NAME |
|
NAME: Boundary
Group name to be created, modified or deleted |
|
*LOAD-GROUP (Load
Group) |
|
Grouping nodes or elements assigned with
loads by
assigning a specific load group name |
|
; NAME |
|
NAME: Load
Group name to be created, modified or deleted |
|
*USE-STLD |
|
Corresponding unit load case
USE-STLD: shows
entered unit load cases and the coresponding loads |
|
*SELFWEIGHT
(Self Weight) |
|
Applying the selfweight of the analysis
model as loads |
|
; *SELFWEIGHT, X, Y, Z,
GROUP |
|
X: weight
scale factor for the X-direction component in GCS
Y: weight
scale factor for the Y-direction component in GCS
Z: weight
scale factor for the Z-direction component in
GCSGROUP: Group
Name |
|
*CONLOAD
(Nodal Loads) |
|
loads assigned to nodes |
|
; NODE_LIST, FX, FY, FZ,
MX, MY, MZ, GROUP |
|
NODE_LIST: node
numbers
FX: concentrated
load component in the GCS X-direction
FY: concentrated
load component in the GCS Y-direction
FZ: concentrated
load component in the GCS Z-direction
MX:
concentrated moment component about the GCS X-direction
MY: concentrated
moment component about the GCS Y-direction
MZ:
concentrated moment component about the GCS X-direction
GROUP: Group
Name |
|
*SPOISP (Specified
Displacement of Supports) |
|
Forced displacements of supports |
|
; NODE_LIST, FLAG, Dx,
Dy, Dz, Rx, Ry, Rz, GROUP |
|
NODE_LIST: node
numbers
FLAG: symbol
of degree of freedom to which a specified
displacement will be specified
(6 Digit Code using "1"
or "0")
Dx: specified
displacement component in the X-direction
Dy:
specified displacement component in the Y-direction
Dz:
specified displacement component in the Z-direction
Rx:
specified rotational displacement component about the X-direction
Ry: specified
rotational displacement component about the Y-direction
Rz: specified
rotational displacement component about the Z-direction
GROUP: Group
Name |
|
*BEAMLOAD (
Element Beam Loads ) |
|
Beam loads applied to beam elements |
|
; ELEM_LIST, CMD, TYPE,
DIR, bPROJ, D1, P1, D2, P2, D3
P3, D4, P4, GROUP |
|
ELEM_LIST: element
numbers
CMD: load
classification {BEAM}
= BEAM: Element Beam Load
= FLOOR: Floor Load
= LINE: Line Beam Load
= TYPICAL: Typical Loads
TYPE: load
type {UNILOAD}
= CONLOAD: Concentrated
Forces
= CONMOMENT: Concentrated
Moments
= UNILOAD: Uniform Loads
= UNIMOMENT: Uniform Moments/Torsions
DIR: direction
of load {GZ}
LX: X-direction
in the element local coordinate system
LY: Y-direction
in the element local coordinate system
LZ: Z-direction
in the element local coordinate system
GX: about
X-direction in GCS
GY: about
Y-direction in GCS
GZ: about
Z-direction in GCS
bPROJ: option
to specify projection of beam loads {NO}
(not relevant to concentrated
loads or concentrated moments)
D1:
location of beam load on the beam element
P1:
magnitude of the beam load
GROUP:Group
Name |
|
*FLOADTYPE(Define
Floor Load Type ) |
|
Definition of floor load |
|
; NAME, DESC ;
1st line
; LCNAME1, FLOAD1, bSBU1,
..., LCNAME4, FLOAD4,
;
2nd line |
|
NAME: name
of floor load
DESC: brief
description
LCNAME1: name
of unit load case
FLOAD1: magnitude
of unit load
option
to to include the weight of dummy beam elements (YES/NO)
|
|
*FLOAD-COLOR |
|
Color data of floor loads |
|
; NAME, W_R, W_G, W_B,
HF_R, HF_G, HF_B, HE_R, HE_G
HE_B, bBLEND, FACT |
|
NAME:
name of floor load
W_R: red
color number when displaying in Wire Frame
W_G:
green color number when displaying in Wire Frame
W_B: blue
color number when displaying in Wire Frame
HF_R:
red color number of Hidden treated surface
HF_G:
green color number of Hidden treated surface
HF_B: blue
color number of Hidden treated surface
HE_R:
red color number of the outline of Hidden treated surface
HE_G: green
color number of the outline of Hidden treated surface
HE_B: blue
color number of the outline of Hidden treated surface
bBLEND: assigns
color transparency
(YES/NO) {NO}
FACT: factor
(degree) of color transparency {0.5} |
|
*FLOORLOAD (Floor
Loads) |
|
load (floor load) onto beam or
wall elements within an enclosed range |
|
; LTNAME, iDIST, ANGLE,
iSBEAM, SBANG, SBUW, DIR,
bPROJ, DESC, GROUP, NODE1,
..., NODEn |
|
LTNAME: name
of floor load
iDIST: method
of distributing floor load {2}
= 1 : distributed in 1
direction
= 2 : distributed in 2
directions
= 3 : Polygon-Centroid
= 4 : Polygon-Length
ANGLE: angle
of the direction of the load distribution {0}
iSBEAM: number
of imaginary sub-beams placed in a sub-area {0}
SBANG: placement
angle of the imaginary sub-beams {90}
SBUW:
self-weight per unit length of a sub-beam [load/length] {0}
DIR: acting
direction of floor load {GZ}
LX: X-direction
in the local floor coordinate system
LY: Y-
direction in the local floor coordinate system
LZ: Z-direction
in the local floor coordinate system
GX: X-direction
in GCS
GY:
Y-direction in GCS
GZ: Z-direction
in GCS
bPROJ: option
to specify projection of floor loads (YES/NO) {NO}
DESC: brief
description
GROUP:
Group Name
NODE1, ..., NODEn:
node numbers identifying the floor load |
|
*PRESTRESS (Prestress Beam Loads ) |
|
Prestress loads |
|
; ELEM_LIST, LTYPE, TENS,
DI, DM, DJ, GROUP |
|
ELEM_LIST: element
numbers
LTYPE: type
of beam element prestress load {1}
(not relevant to truss/tension-only/compression-only
elements)
= PRE: process of prestress
effect is considered
(Prestress condition)
= POST: condition after
the prestress is considered
(Post-stress condition)
TENS: Prestress
Tension Force
DI:
Cable Drape in the ECS z-direction at the i-node of the beam element
DM:
Cable Drape in the ECS z-direction at the center point of the beam element
DJ: Cable
Drape in the ECS z-direction at the j-node of the beam element
GROUP: Load
Group Name |
|
*PRETENSION (Pretension
Loads) |
|
Pretension Loads |
|
; ELEM_LIST, TENS, GROUP |
|
ELEM_LIST : element
numbers
TENS:
Pretension Load
GROUP:
Load Group Name |
|
*FINISHINGLOADS (Finhing
Material Loads) |
|
Finishing Loads |
|
; ELEM_LIST, COVERING-TYPE,
FACE1, FACE2, FACE3,
FACE4, D, DENSITY, DIR,
SCALE, GROUP
; *SYSTEMP*PRESSURE ;
Pressure Loads
; ELEM_LIST, CMD, ETYP,
LTYP, DIR, VX, VY, VZ, bPROJ
PU, P1, P2, P3, P4, GROUP
;
ETYP=PLATE, LTYP=FACE
; ELEM_LIST, CMD, ETYP,
LTYP, iEDGE, DIR, VX, VY, V
PU, P1, P2, GROUP ;
ETYP=PLATE, LTYP=EDGE
; ELEM_LIST, CMD, ETYP,
iEDGE, DIR, VX, VY, VZ, PU, P1
P2, GROUP ;
ETYP=PLANE
; ELEM_LIST, CMD, ETYP,
iFACE, DIR, VX, VY, VZ, bPROJ,
PU, P1, P2, P3, P4, GROUP
;
ETYP=SOLID
; [PLATE] : plate, plane
stress, wall, [PLANE]
: axisymmetric, plane
strain
ER, SYSTEMP, GROUP |
|
ELEM_LIST: element
numbers
COVERING-TYPE: assigns
the method of applying finishing loads
= ENVELOP
= FILL
= SURROOND
FACE 1~4: assigns
the range of finishing material
=
FULL
=
HALF
D: thickness
of finishing
DENSITY: unit
weight of the finishing material
DIR:
direction of the finishing material load
= Gx: X-direction in GCS
= Gy: Y-direction in GCS
= Gz: Z-direction in GCS
SCALE: scale
factor for applying the finishing load |
|
*PRESSURE (Pressure
Loads) |
|
Pressure loads |
|
; ELEM_LIST, CMD, ETYP,
LTYP, DIR, VX, VY, VZ, bPROJ
PU, P1, P2, P3, P4, GROUP
;
ETYP=PLATE, LTYP=FACE
; ELEM_LIST, CMD, ETYP,
LTYP, iEDGE, DIR, VX, VY, VZ
PU, P1, P2, GROUP ;
ETYP=PLATE, LTYP=EDGE
; ELEM_LIST, CMD, ETYP,
iEDGE, DIR, VX, VY, VZ, PU, P1
P2, GROUP ;
ETYP=PLANE
; ELEM_LIST, CMD, ETYP,
iFACE, DIR, VX, VY, VZ, bPROJ
PU, P1, P2, P3, P4, GROUP
; ETYP=SOLID
; [PLATE] : plate, plane
stress, wall, [PLANE]
: axisymmetric, plane
strain
ER, SYSTEMP, GROUP |
|
1. Common items
ELEM_LIST: element
numbers
CMD: type
of load
= PRES: Pressure Loads
= HYDRO: Hydrostatic Pressure
Loads
ETYP: selects
the type of element {PLATE}
= PLATE: Plate
= PLANE: Plane Stress,
Plane Strain, Axisymmetric
= SOLID:
8 Node-Solid, 6 Node-Solid, 4 Node-Solid
2. If ETYPE
is ‘PLATE’ and LTYPE is ‘FACE’
LTYPE: location
of loading application {FACE}
DIR: direction
of load application
= Lx, Ly, Lz: loading
applied in x, y, z ditrections in ECS
= Gx, Gy, Gz: loading
applied in X, Y, Z ditrections in GCS
= VECTOR:
loading applied in the direction of the vector defined
by User
Vx, Vy, Vz:
X, Y, Z-direction distances defining the vector from the
reference point in GCS
bPROJ: option
to specify projection of loads {NO}
PU: Uniformly
distributed load value
P1~4: Linearly
distributed load value
GROUP: Load
Group name
3. If ETYPE
is ‘PLATE’ and LTYPE is ‘EDGE’
LTYPE:
location of loading application {FACE}{EDGE}
iEDGE: element
edge subjected to load application
= 1 : EDGE #1
= 2 : EDGE #2
= 3 : EDGE #3
= 4 : EDGE #4
: direction of load application
= NORMAL: loads applied
in the direction paralleled with the
element face
*for others: refer to
#2 above
4. If ETYPE
is ‘PLATE’
DIR:
direction of load application
= NORMAL, Lx, Ly, Vector:
refer to #2 & #3
5. If ETYPE
is ‘SOLID
iFACE: element
face onto which the load is applied
= 1 : Face #1
= 2 : Face #2
= 3 : Face #3
= 4 : Face #4
= 5 : Face #5
= 6 : Face #6
**for others: refer to
#2, #3 & #4 above |
|
*SYSTEMPER (System
Temperature) |
|
Final temperature in thermal stress analysis |
|
; *SYSTEMPER, SYSTEMP,
GROUP |
|
SYSTEMP: final
temperature of structure
GROUP:
Load Group Name |
|
*NDTEMPER (Nodal
Temperatures ) |
|
Nodal temperature at specific nodes |
|
; NODE_LIST, TEMPER, GROUP |
|
NODE_LIST: node
numbers
TEMPER:
nodal temperature
GROUP: Load Group Name |
|
*ELTEMPER (Element
Temperatures) |
|
Element temperature of specific elements |
|
; ELEM_LIST, TEMPER, GROUP |
|
LEM_LIST: element
numbers
TEMPER:
element temperature
GROUP: Load
Group Name |
|
*BSTEMPER (Beam
Section Temperature) |
|
Beam Section Temperature |
|
; ELEM_LIST, DIR, NUM,
GROUP ;
line 1
; TYPE1,
ELAST1, THERMAL1, B1, H11, T11, H21,
T21 ;
line 2
; ...
; TYPEn,
ELASTn, THERMALn, Bn, H1n, T1n, H2n, T2n
;
line n+1 |
|
ELEM_LIST: element
numbers
DIR:
input direction of beam section temperature load
NUM: number
of temperature loads entered
GROUP: Load
Group Name
TYPE1:
material property to be applied
ELAST1: modulus
of elasticity
THERMAL1: thermal
expansion coefficient
B1: width
to be considered for temperature difference
H11, H21: distance
from the centroid to the point of the temperature application
T11, T21: temperatures
at H11 & H21 |
|
*THERGRAD (Temperature Gradient) |
|
Temperature gradient (difference) between
the
upper and lower faces of a beam or plate
element |
|
; ELEM_LIST, iETYP, TZ,
bUSEHZ, HZ, TY, bUSEHY, HY, GROUP
; ELEM_LIST, iETYP, TZ,
bUSEHZ, HZ, GROUP |
|
ELEM_LIST: element
number
iETYP: element
type {1}
= 1 : beam element
= 2 : plate element
. In the case of beam element
TZ: temperature
difference between the two outer faces in the
element
local z-direction
bUSEHZ: option
to use member dimensions (YES/NO) {YES}
HZ: distance
between the two outer faces in the element local z-direction
TY:
temperature difference between the two outer faces in the
element local y-direction
bUSEHY:
option to use member dimensions (YES/NO) {YES}
HY: distance
between the two outer faces in the element local y-direction
GROUP:
Load Group Name.
In the case of plate element
TZ:
temperature difference between the two outer faces in the
element local z-direction
bUSEHZ: option
to use member dimensions (YES/NO) {YES}
HZ: thickness of plate element |
|
*WIND (Wind
Loads) |
|
Wind loads |
|
; CODE=CODE, SFX, SFY,
ESC
;
line 1
; [KS1992] :
EC, BWS, PC
;
line 2
; [JP1987] :
PRF, WPC
;
line 2
; [UBC1997] :
EC, BWS, IF, PC
;
line 2
[ANSI1982] :
EC, BWS, IF, WC, LC
;
line 2
; [KS2000] :
EC, GF, BWS, IF, HROOF, KZT, HZT
;
line 2
; [IBC2000] :
iPROC, EC, GFX, GFY, BWS, IF, HROOF,
TF, WF, iRIG, iENC, RF
;
line 2
[EURO1992] :
iPROC, RC, RWS, SCC, FORC,
FRIC, TOPO, GRF ;
line 2
; [BS6399(97)]: iPROC,
SC, KB, VB, HO, X, CF, SD, TD,
SA, SD, SS, SP, SH ;
line 2
; [CH2001] :
RC, SMT, BWS, MF, WPC, LPC, FPX, FPY
;
line 2
; [JP2000] :
EC, BWS
;
line 2
; [NBC1995] :
iPROC, RWS, GEF, CGX, CGY, BH, EC,
bITE, HS, BL, HH, HL,
CBD ;
line 2
; SSTORY1, ESTORY1, ADDX1,
ADDY1, ...
;
from line 3 |
|
CODE: select
a code to be applied to wind load calculation
= IBC2000,
UBC1997, ANSI1982, NBC1995, EURO1992, BS6399
SFX: scale
factor applied to X-direction in GCS
SFY: scale
factor applied to Y-direction in GCS
DESC:
brief description
In the case of [KS1992]
EC: exposure
category : 'A', 'B', 'C' {B}
BWS: basic
wind speed (unitless) {30}
PC: wind
pressure coefficient {1.4}
In the case of [JP1987]
PRF:
wind pressure reduction factor {0}
WPC: wind
pressure coefficient {0}
In the case of [UBC1997]
EC: exposure
category : 'B', 'C', 'D' {B}
BWS:
basic wind speed (unitless) {80mile/h}
IF: importance
factor {1}
PC: wind
pressure coefficient {1.3}
In the case of [ANSI1982]
EC: exposure
category: 'A', 'B', 'C', 'D' {A}
BWS: basic
wind speed (unitless) {80mile/h}
IF: importance
factor {1}
WC: Windward
wind pressure coefficient {0.8}
LC: Leeward
wind pressure coefficient {0.5}
In the case of [KS2000]
EC: exposure
category: 'A', 'B', 'C', 'D' {B}
GF: Gust
factor
BWS: basic
wind speed (unitless) {30}
IR:
importance factor
HROOF: average
roof height
KZT: wind
speed scale factor for topography
HZT: vertical
height for wind speed factor
In the case of [IBC2000]
iPROC: calculation
method for wind load
= 1: Simplified Procedure
= 2 : Analytical Procedure
EC: exposure
category: ‘B’, ‘C’, ‘D’, {B}
GFX:
Gust Factor X
GFY: Gust
Factor Y
BWS: basic
wind speed {30mile/h}
IF:
importance factor {1.0}
HROOF:
mean roof height
WF: wind
directionality factor
iRIG:
structural rigidity
= 0 : Rigid Structure
= 1 : Flexible Structure
In the case of [EURO1992]
iPROC: calculation
method for wind load
= 1: Simplified Method
= 2
: Detailed Method
RC: roughness
category: ‘1’, ‘2’, ‘3’, ‘4’,
{1}
RWS: reference
wind speed {24.5m/sec}
SCC: size
coefficient
FORC:
force coefficient
FRIC: friction
coefficient
TOPO:
topography coefficient
GRF: gust
response factor
In the case of [BS6399(97)
]iPROC: calculation
method for wind load
= 1: Standard Method
= 2 : Directional Method
SC: site
category (COUNTRY /TOWN)
KB: building
type factor {1}
VB: basic
wind speed {24m/sec}
HO: mean
roof height
X: separation
of building
CF: friction
drag coefficient
SD: closet
diatance to sea
DTdistance
to town edge
SA:
altitude factor:
SD: directional
factor
SS: seasonal
factor
SP:
probability factor
SH: topographic
increment
In the case of [CH2001]
RC: roughness
category : ‘A’, ‘B’, ‘C’, ‘D’,
{A}
SMT: structural
meterial type
=
ST: Steel
= SW: Steel + Infilled
Wall
= RC: RC
BWS: basic
wind pressure
MF:
modification factor for
WPC: windward
pressure coefficient
LPC: leeward
pressure coefficient
FPX: fundamental
period of the structure in the X-direction
FPY: fundamental
period of the structure in the Y-direction
In the case of [JP2000]
EC: exposure
category : ‘¥°’,
‘¥±’, ‘¥²’, ‘¥³’, {¥°}
BWS:
basic wind speed {32m/sec}
In the case of [NBC1995]
iPROC: calculation
method for wind load
= 1: Simple Procedure
= 2 : Detailed Procedure
RWS: reference
wind speed {30m/sec}
GEF: Gust
factor (Simple Procedure)
CGX: Gust
factor (Detailed Procedure)
CGY: Gust
factor (Detailed Procedure)
BH: building
height
EC: exposure
category : ‘A’, ‘B’, ‘C’, {A}
BITE: option
to consider the wind speed scale factor according to to
pography {NO}
HS: hill
shape
= 2DR : 2-D Ridge or Valley
(mountain)
= 2DE : 2-D Escarpment
(slope)
= 3DA : 3-D Axisym. Hill
(hill)
BL: building
location - building location in case 2-D Escarpment
HH: hill
height - height of the hill or the difference in elevation between
the crest of the hill
and that of the terrain surrounding the upstream
HL:
hill length - distance upwind of the crest to where the ground elevation
is half
the height of the hill
CBD: crest-building
distance
SSTORY1: start
story for applying additional wind load
ESTORY1: end
story for applying additional wind load
ADDX1: additional
wind load in the global X-direction
ADDY1: additional
wind load in the global Y-direction |
|
*SEIS (Static
Seismic Loads) |
|
Equivalent Static Seismic Loads |
|
; CODE=CODE, SFX, SFY,
ECCX, ECCY, DESC
;
line 1
; [KS1992] :
SPT, EA, IF, PAX, PAY, PCX, PCY, RMFX,
RMFY ;
line 2
; [UBC1991] : SPT, ZF,
IF, PAX, PAY, PCX, PCY, NCX,
NCY ;
line 2
; [UBC1997] : SPT, ZF,
SST, CD, IF, PX, PY, NCX,
NCY ;
line 2
; [ATC306] :
SPC, EPV, PAX, PAY, PCX, PCY, RMFX,
RMFY ;
line 2;
[KS2000] :
SPT, EA, IF, PAX, PAY, PCX, PCY, RMFX,
RMFY ;
line 2
; [JIS] :
SPT, EA, SF, PAX, PAY, PCX, PCY, RMFX,
RMFY ;
line 2
; [IBC2000] : SDC, SC,
MS, M1, IF, PX, PY, PCX, PCY, RMFX,
RMFY ;
line 2
; [EURO1996]: S, QO, KD,
KR, KW, ALPHA, FPX,
FPY ;
line 2
; [CH2001] :
NSC, SFI, SC, ST, DR, EQ, bMM, FPX
FPY ;
line 2
; [NBC1995] : ZVR, AZ,
VZ, IF, FF, PAX, PAY, PCX, PCY,
FMFX, FMFY
;
line 2
; SSTORY1, ESTORY1, ADDX1,
ADDY1, ...
;
from line 3 |
|
CODE: select
a code to be applied to seismic load calculation
= IBC2000,
UBC1997, UBC1991, ATC306, NBC1995, EURO1996
SFX:
scale factor applied to X-direction in GCS
SFY:
scale factor applied to Y-direction in GCS
ECCX: accidental
eccentricity torsion induced by the story seismic
load
in the X-direction in
GCS
= POS: counter-clockwise
= NEG: clockwise
ECCY: accidental
eccentricity torsion induced by the story seismic
load
in the Y-direction in
GCS
= POS: counter-clockwise
= NEG: clockwise
DESC: brief
description
In the case of [KS1992]
SPT: soil
profile type (= 1.0, 1.2, 1.5) {S2(1.2)}
EA: earthquake
area factor (= 0.08, 0.12) {Area2(0.12)}
IF: importance
factor (= 0.8, 1.0, 1.2, 1.5) {1.2}
PAX: natural
period in the X-direction obtained by the eigenvalue analysis {0}
PAY: natural
period in the Y-direction obtained by the eigenvalue analysis {0}
PCX: natural
period in the X-direction obtained by the code {0}
PCY:
natural period in the Y-direction obtained by the code {0}
RMFX:
response modification coefficient in X-direction {6}
RMFY:
response modification coefficient in Y-direction {6}
In the case of [UBC1991]
SPT: soil
profile type (= 1.0, 1.2, 1.5) {S1(1.0)}
ZF: seismic
zone factor (= 0.075, 0.15, 0.2, 0.3, 0.4) {0.075}
IF: importance
factor (= 1.0, 1.25) {1.0}
PAX:
natural period in the X-direction obtained by the eigenvalue analysis
{0}
PAY: natural
period in the Y-direction obtained by the eigenvalue analysis {0}
PCX:
natural period in the X-direction obtained by the code {0}
PCY:
natural period in the Y-direction obtained by the code {0}
NCX:
ductility coefficient : numerical coefficients representative of the
inherent overstrength
and global ductility capacity of a lateral force
resisting system in the
X-direction
NCY:
ductility coefficient : numerical coefficients representative of the
inherent overstrength
and global ductility capacity of a lateral force
resisting system in the
Y-direction
In the case of [UBC1997]
SPT: soil
profile type (= Sa, Sb, Sc, Sd, Se, Sf) {Sa}
ZF: seismic
zone factor (= 0.075, 0.15, 0.2, 0.3, 0.4) {0.075}
SST: seismic
source type {A}
CD: closest
distance to known seismic source {10 KM}
IF:
importance factor
PX: natural
period in the X-direction obtained by the eigenvalue analysis
PY: natural
period in the Y-direction obtained by the eigenvalue analysis
NCX: ductility
coefficient : numerical coefficient relative to structural
ductility and over-strength
in the X-direction
NCY: ductility
coefficient : numerical coefficient relative to structural
ductility and over-strength
in the Y-direction
In the case of [ATC306]
SPC: soil
profile coefficient{0}
EPV: effective
peak velocity{0}
PAX: natural
period in the X-direction obtained by the eigenvalue analysis {0}
PAY: natural
period in the Y-direction obtained by the eigenvalue analysis {0}
PCX:
natural period in the X-direction obtained by the code {0}
PCY:
natural period in the Y-direction obtained by the code {0}
RMFX: response
modification factor in X-direction
RMFY: response
modification factor in Y-direction
In the case of [KS2000]
SPT: soil
profile type (= 1.0, 1.2, 1.5) {S2(1.2)}
EA: earthquake
area factor (= 0.07, 0.11) {Area1(0.11)}
IF: importance
factor (= 0.8, 1.0, 1.2, 1.5) {1.2}
PAX: natural
period in the X-direction obtained by the eigenvalue analysis {0}
PAY: natural
period in the Y-direction obtained by the eigenvalue analysis {0}
PCX: natural
period in the X-direction obtained by the code {0}
PCY: natural
period in the Y-direction obtained by the code {0}
RMFX: response
modification coefficient in X-direction {6}
RMFY:
response modification coefficient in Y-direction {6}
In the case of [JIS]
SPT:
soil period {0.6sec (¥±)}
EA: seismic zone
factor
SF:
base shear factor
PAX:
natural period in the X-direction obtained by the eigenvalue analysis
{0}
PAY:
natural period in the Y-direction obtained by the eigenvalue analysis
{0}
PCX: natural
period in the X-direction obtained by the code {0}
PCY:
natural period in the Y-direction obtained by the code {0}
RMFX:
response modification coefficient in X-direction
RMFY:
response modification coefficient in Y-direction
In the case of [IBC2000]
SDC: seismic
design categories : ‘A’,
‘B’, ‘C’, ‘D’, ‘E’, ‘F’,
{A}
SC: soil
class : ‘A’, ‘B’, ‘C’, ‘D’, ‘E’,
{A}
MS: mapped
spectral response acceleration at short periods {0.25}
M1: mapped
spectral response acceleration at 1 second periods {0.1}
IF:
Importance factor {1.0}
PX, PY: natural
period obtained by eigenvalue analysis
PCX, PCY: natural
period obtained by the formula in the code
RMFX, RMFY: response
modification coefficient
In the case of [EURO1996]
S: soil
class {A(1.0)}
QO: basic
behavior factor based on structure type {5.0}
KD: ductility
class {High (1.00)}
KR: elevation
regularity {Regular (1.00)}
KW: failure
mode factor {1}
ALPHA: ratio
of design ground acceleration to gravity acceleration
FPX, FPY: fundamental
period
In the case of [CH2001]
NSC: near
source category {1}
SFI: seis.
fortification intensity {6(0.05g)}
SC: site
class {1}
ST: structure
type
= RSM: RC or Steel Multistory
= IFM: Interior Framed
Multistory
= TSB: Tall Steel Building
(JGJ99-98)
= ETC: Etc
DR: damping
ratio
EQ: Earthquake
frequency
= FREQUENT: frequent earthquake
(weak)
= SCARCE: scarce earthquake
(strong)
Bmm: whether
or not masonry structure type is applied : masonry
multistory, framed 1st
story, interior frame - exterior masonry structure
FPX, FPY:
fundamental period
In the case of [NBC1995]
ZVR: zonal
velocity ratio {0.05}
AZ:
acceleration zone : acceleration related seismic zone{1}
IF: importance
factor {1}
FF:
foundation factor {1}
PAX, PAY: natural
period obtained by eigenvalue analysis
PCX, PCY: natural
period obtained by the formula in the code
FMFX, FMFY: force
modification factor for each direction
SSTORY1: start
story of additional seismic load to be applied
ESTORY1:
end story of additional seismic load to be applied
ADDX1:
additional seismic load value in the X-direction in GCS
ADDY1: additional
seismic load value in the Y-direction in GCS |
|
*TDN-PRESTRESS (Tendon
Prestress Loads) |
|
Apply tendon prestress loads |
|
; TDN-NAME, FORCE/STRESS,
JACKING, BEGIN, END,
iGROUTING, GROUP |
|
TDN-NAME:
tendon name to which prestress loads are applied
FORCE/STRESS: input
tension force in force/stress units
JACKING: order
of tentioning tendons
BEGIN:
tension force at the start of tendon
END: tension
force at the end of tendon
iGROUTING: timing
of grrouting duct
GROUP:
load group for tendon prestress loads (Load Group Name) |
|
*TIMELOAD (Time
Load) |
|
Tme dependent property due to the difference
in
member ages |
|
; ELEM_LIST, DAY, GROUP |
|
ELEM_LIST: element
numbers subjected to Time Load
DAY: member
age
GROUP: Load
Group Name |
|
*CREEPCOEF |
|
Creep coefficient directly input in the
form of load |
|
; ELEM_LIST, CREEP, GROUP |
|
ELEM_LIST: element
numbers for which the creep coefficient is considered
CREEP: creep
coefficient
GROUP:
Load Group Name |
|
*PNLOADTYPE (Plane
Load Type) |
|
Type and size of plane load |
|
; NAME=NAME, TYPE(POINT/LINE/AREA),
DESC
; CP_X=X1, X2, ...
; CP_Y=Y1, Y2,
; DATA=X1,
Y1, F1, M1 ;
T Y P E = P O I N T
; ...
; Xn,
Yn, Fn, Mn
; DATA=bUNIFORM, TYPE,
X1, Y1, L1, X2, Y2, L2
;
TYPE=LINE
; DATA=bUNIFORM, b3PT,
X1, Y1, L1, X2, Y2, L2, X3, Y3, L3
X4, Y4, L4 ;
TYPE=AREA |
|
NAME: name
of plane load
TYPE(POINT/LINE/AREA):
type of load
DESC:
brief description
CP_X: copy
distance in the x-direction of the plane coordinat
system
for loading simultaneous plane loads
CP_Y: copy
distance in the y-direction of the plane coordinate
system
for loading simultaneous plane loads
1. In the case of POINT
X1: x-coordinate
of the location of loading application
Y1: y-coordinate
of the location of loading application
F1:
magnitude of the concentrated load
M1: magnitude
of the concentrated moment
2. In the case of LINE
bUNIFORM: option
to apply a uniformly distributed load
TYPE:
assigns the load type
X1, X2: x-coordinate
of the entered load
Y1, Y2: y-coordinate
of the entered load
L1, L2: magnitude
of the entered load
3. In the case of AREA
bUNIFORM: option
to apply a uniformly distributed load
X1, X2, X3, X4: x-coordinate
of the entered load
Y1, Y2, Y3, Y4: y-coordinate
of the entered load
L1, L2, L3, L4:
magnitude of the entered load |
|
*PLANELOAD (Plane
Load) |
|
Applying Plane load to any point on plate
and solid elements |
|
; LCNAME, LTNAME, ETYPE,
GROUP
;
1st line
; ELEM-SEL, ELEM-GROUP,
FACE, DIR, PROJ, DESC
;
2nd line
; OX, OY, OZ, XX, XY,
XZ, YX, YY, YZ, TOL, bLAREA
iNODE1, ... , iNODEn ;
3rd line |
|
LCNAME:
name of unit load case
LTNAME: name
of plane load
ETYPE:
type of the selected elements (Plate/Solid)
DIR: direction
of the plane load application
bPROJ: option
to apply the projectied area
DESC:
brief description
GROUP:
Load Group Name
OX, OY, OZ: coordinates
of the origin point of the plane local coordinate system
XX, XY, XZ: coordinates
on the x-axis in the plane local coordinate system
YX, YY, YZ: coordinates
on the y-axis in the plane local coordinate system
TOL: coordinate
tolerance of a point
bLAREA: select
whether or not to assign the loaded area
iNODE1:
node numbers defining the outline of plane load |
|
*INIF-CTRL (Initial Force Control Data) |
|
Saving the initial axial force as the results
of a separate load case |
|
; bADD, LOADCASE |
|
bADD: option
to enter the initial axial force as the results of a
separate
load case (YES/NO) {NO}
LOADCASE: load
case, which will save or add initial axial force |
|
*INIFORCE (Initial
Forces for Geometric Stiffness ) |
|
Entering initial axial forces required
to calculate the
geometric stiffness of specific members |
|
; ELEM_LIST, DIR, FORCE |
|
ELEM_LIST: element
numbers for which initial axial forces are entered
DIR: direction
of initial axial force
= AXIAL: applies the force
as the element’s axial force
= GX:
considers the force in the global X-direction, such that the
axial forces for the object
elements are automatically calculated and
entered relative to their
orientations
= GY
= GZ
FORCE: magnitude
of axial force |
|
*SFUNCTION (Specturm
Function) |
|
Spectrum data required for response spectrum
analysis |
|
; FUNC=NAME, iTYPE, SCALE,
GRAV, DESC ;
line 1
; PERIOD1, VALUE1, PERIOD2,
VALUE2, ... ;
from line 2 |
|
FUNC:
name of spectrum data
iTYPE:
assigns data type {1}
= 1 : Normalized Acceleration
= 2 : Acceleration
= 3 : Velocity
= 4 : Displacement
SCALE: correction
factor for spectrum data {1}
GRAV: gravitational
acceleration {9.806 m/sec2
DESC: brief
discription
PERIOD1:
period value
VALUE1: value
of spectrum data |
|
*SPLDCASE (Spectrum
Load Cases) |
|
Basic data required for response spectrum
analysis
(load case) |
|
; NAME, FUNC, DIR, ANGLE,
SCALE, DESC |
|
NAME:
name of response spectrum analysis case
FUNC: spectrum
function to be applied to response spectrum analyis
DIR: applied
direction of spectrum load {XY}
XY:
lateral directions of the structure
Z: vertical
direction of the structure
ANGLE: input
angle of seismic load with respect to the X-direction
of GCS if X-Y plane selected
(right hand sign convention
about the Z-axis) {0}
SCALE: scale
factor for input loads {1}
DESC: brief
description |
|
*TFUNCTION (Time
History Function) |
|
Time history load function |
|
; FUNC=NAME, 1, iTYPE,
SCALE, GRAV, DESC
;
line 1
; TIME1, VALUE1, TIME2,
VALUE2, ... ;
from line 2
; FUNC=NAME, 2, iTYPE,
GRAV, A, C, F, D, PA, DESC |
|
NAME: name of time history function
iTYPE: assigns
the type of data {1}
= 1 : Normalized Acceleration
= 2 : Acceleration
= 3 : Force
= 4 : Moment
For 1 (=Time
History Function )
SCALE:
the scale factor of data{1}
GRAV: gravitational
acceleration {9.806 m/sec2}
DESC: brief
discription
TIME1: time
VALUE1: time
history load data
For 2 (= Sinusoidal Function) {0}
A, C:
constantsF:
F:frequency
of the input load [Cycle/sec]
D: damping
coefficient
PA: phase
angle |
|
*THLDCASE (Time
History Load Cases) |
|
Basic data required for executing time
history analysis
(load
case) |
|
; NAME=NAME, DESC ;
line 1 |
|
NAME:
name of the load case of the time history function
DESC: brief
descriptionn
ETIME: end
time of the time history analysis {1sec}
INC:
time increment of the time history analysis (0.1 sec)
iOUT: analysis
interval required for producing the time history analysis results {1}
iMODE1: mode
number {0}
DAMPING1: damping
coefficient for each mode {0}
DALL: damping
coefficient used for all the modes {0} |
|
*DYN-NLOAD
(Dynamic Nodal Loads) |
|
Applying a time history function to nodes
in a specific direction |
|
; NODE_LIST, THIS, FUNC,
DIR, ARTIME, SCALE |
|
NODE_LIST: node
numbers
THIS: selects
the time history analysis condition
FUNC:
type of time load function
DIR:
loading direction of the time load function {X}
= X, Y, Z
ARTIME: arrival
(delay) time for the time load function {0sec}
SCALE: scale
factor for the time load function {1} |
|
*GROUND-ACC |
|
Specifying a time load function as a ground
acceleration |
|
; THIS, FUNCX, SCALEX,
ATIMEX, FUNCY, SCALEY,
ATIMEY,
FUNCZ, SCALEZ, ATIMEZ, |
|
THIS: selects
the time history analysis condition
1. Ground acceleration in the X-direction
of the GCS
FUNCX: selected
time load function from the list
SCALEX: scale
factor for the time load function {1}
ATIMEX: arrival
(delay) time for the time load function {0}
2. Ground acceleration in the Y-direction
of the GCS
FUNCY: selected
time load function from the list
SCALEY: scale
factor for the time load function {1}
ATIMEY:
arrival (delay) time for the time load function {0}
3. Ground acceleration in the Z-direction
of the GCS
FUNCZ: selected
time load function from the list
SCALEZ:
scale factor for the time load function {1}
ATIMEZ: arrival
(delay) time for the time load function {0} |
|
*DYN-SLOAD
(Time Varing Static Load) |
|
Converting static load into time history
load |
|
; THIS, SLOAD, FUNC, ATIME,
SCALE |
|
THIS: selects
the time history analysis condition
SLAOD: Static
Load condition
FUNC:
name of the Time History Load Function
ATIME: arrival
time of the Time History Load Function {0sec}
SCALE:
scale factor of the Time History Load Function {1} |
|
*TH-GRAPH |
|
Producing time history analysis resuits
in graohs relative to time
(displacements, member forces and stresses
in truss/beam elements |
|
; NAME, iENTITY, iFTYPE,
iSTYPE, iPOS, iCOMP, bALL,
iSEL, iOPT, |
|
1. Common items
NAME: name
of the graphic output function of the time
history analysis results
iENTITY: node
number of a truss/ beam element
iFTYPE: type
of the time history analysis results to
be produced
= 2 : Displacement
= 3 : Truss Force/Stress
= 4 : Beam Force/Stress
2. In the case of Displacement
iSTYPE: type of the time
history analysis results to be produced in a graph
= 1 : Displ. (displacement)
= 2 : Vel. (velocity)
= 3 : Accel. (acceleration)
iPOS: {1}
iCOMP: direction
component of the displacement
= 1 : DX
= 2 : DY
= 3 : DZ
= 4 : RX
= 5 : RY
= 6 : RZ
bALL: selects
the Modes, which will be reflected in the time history calculation
= YES: All Modes
= NO: One Mode
iSEL: selected
Mode
iOPT: {0}
3. In the case of Truss Force/Stress
iSTYPE: type
of the time history analysis results to be produced
= 1 : Force
= 2 : Stress
iPOS: location
on a truss for which the results will be produced
= 1 : I-Node
= 2 : J-Node
iCOMP:
member force or stress component
= 1 : FX SX
iOPT: {0}
4. In the case of Beam Force/Stress
iSTYPE: type
of the time history analysis results to be produced
= 1 : Force
= 2 : Stress
iPOS: location
on a beam for which the results will be produced
= 1 : I-Node
= 2 : J-Node
iCOMP:
member force or stress component
= 1 : Axial Axial
= 2 : Shear-y Shear-y
= 3 : Shear-z Shear-z
= 4 : Torsion Bend(+y)
= 5 : Moment-y Bend(-y)
= 6 : Moment-z Bend(+z)
iOPT: option
to combine Axial
= 0 : do not consider
= 1 : consider |
|
*LINELANE (Traffic
Line Lanes) |
|
Lane data required for applying traffic
moving loads |
|
; NAME=NAME, LDIST, GROUP,
;
line 1
; iELEM1, ECC1, FACT1,
... ;
from line 2 |
|
NAME:
traffic line lane classification number
LDIST:
assign objects to distribute the traffic load
GROUP: Cross
Beam Element Group
iELEM1: start
element number among the beam element
(or variable section element)
numbers
ECC1: eccentricity
distance from the center of the beam to the traffic line lane {0}
FACT1:
impact factor for the traffic load (0<=FACT<=0.3) {0} |
|
*SURFLANE (Traffic
Surface Lanes) |
|
Traffic surface lane data |
|
; NAME=NAME, WIDTH, START,
END,
;
line 1
; iNODE1, OFFSET1, FACT1,
... ;
from line 2 |
|
NAME: name
of traffic surface lane
WIDTH: width
of the traffic lane {0}
START: slope
at the starting point
END: slope
at the ending point
iNODE1:
node numbers defining the traffic surface lane
OFFSET1: distance
from iNODE1 to the traffic lane center {0}
FACT1:
impact factor for the traffic load (0<=FACT<=3) {0} |
|
*SURFINEL (Plate
Elements for Influence Surface) |
|
Entering plate elements for influence surface
analysis |
|
; ELEM_LIST |
|
ELEM_LIST: element
numbers |
|
*LSUPPORT (Lane
Supports ) |
|
The supports when calculating the max moment
using the
traffic
load ina continuous beam |
|
; ELEM_LIST, |
|
ELEM_LIST: element
number |
|
*LSUPPORT2 (Lane
Supports ?Reactions at Interior Piers) |
|
Assigning the inner points used in moving
load analysis |
|
; NODE_LIST |
|
NODE_LIST: node
numbers of the inner supports |
|
*VEHICLE (Vehicles) |
|
Traffic load |
|
; NAME=NAME, 1
; NAME=NAME, 2,
;
line 1
; LOAD1, DIST1, LOAD1,
DIST2, ... ;
from line 2 |
|
NAME: name
of traffic load
For 1:
Standard
Vehicle Load
* refer to the Table below
For 2
: user defines the traffic
load traffic load by conbining concentrated
traffic loads and traffic
lane loads
uniformly distributed traffic lane load
[force/length] {0}
concentrated
traffic moving load {0}
concentrated traffic moving load used
to calculate bending moment {0}
: concentrated
traffic moving load used to calculate shear force {0}
LOAD1: concentrated
load
DIST1: distance
between concentrated loads |
|
Korean road Standard specification |
DB-24, DB-18, DB-13.5,
DL-24, DL-18, DL-13.5 |
|
Korean standard train loads |
L-25, L-22, L-18, L-15,
S-25, S-22, S-18, S-15,
EL25, EL22, EL18,
HL standard train load,
H15-44, HS15-44, H15-44L, HS15-44L |
|
AASHTO Standard |
H20-44,HS20-44, H20-44L, HS20-44L, AML |
|
Caltrans Standard |
P5, P7, P9, P11,P13 |
|
Other train loads |
CE80(Cooper E80 Train Load),
UIC80(UIC80 Train Load) |
Table 2. Standard traffic loads
|
*VCLASS (Vehicle
Classes ) |
|
Vehicle load group data used for moving
load analysis |
|
; NAME=NAME ;
line 1
VLOAD1, VLOAD2, ... ;
from line 2 |
|
NAME: vehicle
load group
VLOAD1: vehicle
moving load |
|
*MVLDCASE (Moving
Load Cases) |
|
Assigning moving load cases using vehicle
load groups and traffic lanes |
|
; NAME=NAME, SCALE1, SCALE2,
SCALE3, SCALE4,
, DESC ;
1st line
;.VCLASS1, SCALE1, iMIN1,
iMAX1, LANE11,
LANE12, ... ;
2nd line
; ,.VCLASSn, SCALEn, iMINn,
iMAXn, LANEn1
LANEn2, ... ;
th line |
|
NAME:
input the name of moving load condition
SCALE1: reduction
factor used for applying multi-traffic lane loads
{1, 1, 0.9, 0.75}
DESC:
brief description
VCLASS1: select
vehicle load group
SCALE1: scale
factor to be applied to traffic load group {1}
iMIN1: minimum
number of traffic lanes for loading vehicle load group {1}
iMAX1: maximum
number of traffic lanes for loading vehicle load group {1}
LANE11:
selected traffic lanes |
|
*SM-GROUP (Settlement
Group) |
|
Settlement group |
|
; GRNAME, DISPLACEMENT,
NODE_LIST |
|
GRNAME: settlement
group name
DISPLACEMENT:
size of settlement {0}
NODE_LIST:
node number included in the settlement group |
|
*SMLDCASE (Settlement
Load Cases ) |
|
Support settlement group |
|
Support settlement group
;
line 1
GRNAME1, GRNAME2, ...
;
from line 2 |
|
NAME: name
of support settlement
load case
ISMIN::
minimum number of support settlement
groups{1}
ISMAX:
maximum number of support settlement
groups{1}
SCALE : scale
factor for load{1}
DESC : brief
description
GRNAMEL1 :
use of selected support settlement
groups |
|
*SEQUENCE-WZD |
|
Defining the formation of elements and
application
times of loads in construction stages of a structure |
|
; *SEQUENCE-WZD, LCNAME,
DURATION, AGE
; STEP=NO1,
DLSTORY1 ;
line 1
; iTYPE1,
MATL1, MSTORY1, ... ;
from line 2
; ALOAD=LCNAME
;
from here, additional dead load
; SDAY1,
STORY1, ...
; MATL : ALL, STEEL, CONC,
SRC, USER ;
iTYPE=1
; MATL : iMAT ;
iTYPE=2 |
|
LCNAME: unit
load condition applied in the construction stage analysis
DURATION: duration
of the construction stage [day]
AGE: initial
member age of the element [day]
STEP:
construction stage
NO1: sequential
number of the construction stage
DLSTORY1: the
highest story to which the construction load is applied
iTYPE1: method
of defining the element formation in a specific construction stage
= 1: Material Type
= 2: Material Name
1. iTYPE = In case of 1
MATL1:
material applied in the construction load
= ALL
= STEEL
= CONC
= SRC
= USER
2. iTYPE = In case of 2
MATL1: material
number defined
ALOAD:
applied load
LCNAME: unit
load condition applied to the additional load
SDAY1:
start time at which the additional load is applied
STORY1:
the highest story to which the additonal load is applied |
|
*COMPBOXLC
(Load Cases for Pre-composite Section) |
|
Entering pre-composie load case to reflect
the change in
section properties of before and after
composite
action of a composite structural steel
bridge |
|
; LCNAME1, LCNAME2, ...,
LCNAMEn |
|
LCNAME1: load
case to be used as the pre-composite load |
|
*HYD-PRTEMPER (Prescribed
Temperature ) |
|
Entering prescribed temperature condition
for Heat
of hydration analysis |
|
; NODE_LIST, TEMPERATURE,
GROUP |
|
NODE_LIST:
nodes subject to a prescribed temperature
TEMPERATURE: Prescribed
Temperature
GROUP:
Boundary Group |
|
*HYD-PCOOLELEM
(Pipe Cooling) |
|
Entering pipe cooling data intended for
lowering temperature |
|
; NAME=NAME, DIAMETER,
COEF ;
line 1
; HEAT,
DENS, INTEMP, FRATE, iSTART, iEND
;
line 2
; NODE1,
NODE2, NODE3, ... ;
from line 3 |
|
NAME: pipe
cooling group name
DIAMETER: diameter
of cooling pipe
COEF:
convection coefficient
HEAT: specific
heat of water
DENS: density
of water
INTEMP:
water temperature at the inlet
FRATE: flux
per unit time
iSTART:
start time of pipe cooling
iEND: end
time of pipe cooling
NODE1: nodes
defining the course of pipe passage |
|
*HYD-HEATSRCF(Heat
Source Function) |
|
Heat source function applied during hydration |
|
; FUNC=NAME, TYPE, TEMPER
;
TYPE=CONST
; FUNC=NAME, TYPE, K,
ALPHA ;
TYPE=FUNC
; FUNC=NAME, TYPE, SCALE
;
TYPE=USER (line1)
; TIME1, VALUE1, TIME2,
VALUE2, ... ; (from line 2) |
|
1. Common Items
FUNC:
name of heat source function
TYPE: type
of heat sourse function
= CONST: constant value
defined for the heat sourse
= FUNC: code-define heat
source function
= USER: user-defined heat
source values relative to time in a table form
2 In the case of CONST
TEMPER: heat value
3. In the case of FUNC
K: maximum
adiabatic temperature rise
ALPHA:
response speed
4. In the case of USER
SCALE: Scale
Factor
TIME1: time
(hr)
VALUE1: generated
heat value |
|
*HYD-CONVCOEF |
|
Change in convection coefficient at the
convection
boundary surface of a structure |
|
; FUNC=NAME, TYPE, COEFFICIENT
;
TYPE=CONST
; FUNC=NAME, TYPE, SCALE
;
TYPE=USER (line 1)
; TIME1, VALUE1, TIME2,
VALUE2, ... ; (from line 2) |
|
1. Common Items
FUNC:
name of convection coefficient function
TYPE: type
of convection coefficient function
= CONST: convection coefficient
defined as a constant value
= USER: user enters the
convection coefficients relative to time in a table form
2. In the case of CONST
COEFFICIENT: convection
coefficient
3. In the case of USER
SCALE: Scale
Factor
TIME1: time
(hr)
VALUE1: convection
coefficient |
|
*HYD-AMBTEMPF (Ambient
Temperature Function) |
|
Defining the ambient temperature function
to be applied to heat of hydration analysis |
|
; FUNC=NAME, TYPE, TEMPER
;
TYPE=CONST
; FUNC=NAME, TYPE, MAXT,
MEANT, DEALY
;
TYPE=SINE
; FUNC=NAME, TYPE, SCALE
;
TYPE=USER (line 1)
; TIME1, VALUE1, TIME2,
VALUE2, ...
;
(from line 2) |
|
1. Common Items
FUNC: name
of ambient temperature function
TYPE: type
of ambient temperature function
= CONST: ambient temperature
assigned as a constant value
= SINE: ambient temperature
assigned as a Sine function
= USER: user defines the ambient temperature
relative to time
2. In the case of CONST
TEMPER: ambient
temperature
3. In the case of SINE
MAXT: max
amplitude of ambient temperature
MEANT: temperature
immediately after casting
DEALY: delay
day immediately after casting
4. In the case of USER
SCALE:
Scale Factor
TIME1: time(hr)
VALUE1: ambient
temperature |
|
*HYD-HEATSRC (Assign
Heat Source ) |
|
Assigning heat source function to each
element (cast concrete) |
|
; ELEM_LIST, FUNCNAME |
|
ELEM_LIST: element
numbers to be assigned the heat source function
FUNCNAME: selecting
the heat source already entered |
|
*HYD-CONBNDR (Element
Convection Boundary) |
|
Entering heat transfer boundary condition
due to convection |
|
; ELEM_LIST, CCFUNC, ATFUNC,
FACE, GROUP |
|
ELEM_LIST: element
numbers to be assigned the convention
boundary condition
CCFUNC:
selecting the convection coefficient function already entered
ATFUNC:
selecting the ambient temperature function already eneterd
FACE:
defining element surfaces after defining the surface number and assigning
elements
GROUP:
Boundary Group |
|
*HYD-STAGE (Define
Construction Stage For Hydration) |
|
Definition of construction stages in order
to carry out
the construction stage analysis for the
heat of hydration analysis |
|
NAME=NAME ;
line 1
;STEP=DAY1, DAY2, ...
;
line 2
;AELEM=GROUP1, GROUP2,
... ;
line 3
;ABNDR=BGROUP1, BGROUP2,
... ;
line 4
DBNDR=BGROUP1, BGROUP2,
... ;
line 5 |
|
NAME: name
of the constrction stage to be defined
STEP: elapse
time to be defined as Steps within a corresponding construction stage
AELEM: activation
of element groups to define active elements within a corresponding construction
stage
ABNDR: activation
of boundary groups to define active boundart conditions within a corresponding
construction
stage
DBNDR:
defining inactive boundary condition groups |
|
*HINGE-TYPE
(Time Dependent Material) |
|
Defining types of plastic hinges for pushover
analysis |
|
; NAME=NAME, TYPE
; 1st line (TYPE=AXIAL,MOMENT,SHEAR,
PMM)
; NAME=NAME, TYPE, HTYPE,
bSYMMETRIC
; 1st line (TYPE=USER)
; B1P,
B2P (, B1N, B2N)
; 2nd line (TYPE=USER,
HTYPE=AXIAL, PMM, TORSION)
; B1P,
B2P, B3P, B4P(, B1N, B2N, B3N, B4N)
; 2nd line (TYPE=USER,
HTYPE=MOMENT, SHEAR)
; C1P,
C2P (, C1N, C2N)
; 3rd line (TYPE=USER,
HTYPE=AXIAL, PMM, TORSION)
; C1P,
C2P, C3P, C4P (, C1N, C2N, C3N, C4N)
; 3rd line (TYPE=USER,
HTYPE=MOMENT, SHEAR)
; D1P,
D2P (, D1N, D2N)
; 4th line (TYPE=USER,
HTYPE=AXIAL, PMM, TORSION)
; D1P,
D2P, D3P, D4P (, D1N, D2N, D3N, D4N)
; 4th line (TYPE=USER,
HTYPE=AXIAL, PMM, TORSION)
; E1P,
E2P (, E1N, E2N)
; 5th line (TYPE=USER,
HTYPE=AXIAL, PMM, TORSION)
; E1P,
E2P, E3P, E4P (, E1N, E2N, E3N, E4N)
; 5th line (TYPE=USER,
HTYPE=AXIAL, PMM, TORSION)
; IOP,
LSP, CPP (, ION, LSN, CPN)
; 6th line (TYPE=USER)
; bUSECALC
(, YFP, YFN, YDP, YDN)
; 7th line (TYPE=USER,
HTYPE=AXIAL)
; bUSECALC
(, YMYP, PMYN, YMZP, YMZN, YRYPYRYN, YRZP, YRZN)
7th line (TYPE=USE; R,
HTYPE=MOMENT, PMM)
; bUSECALC
(, YFYP, YFYN, YFZP, YFZN, YRYP, YRYN, YRZP, YRZN)
; 7th line (TYPE=USER,
HTYPE=SHEAR)
; bUSECALC
(, YTP, YTN, TRP, YRN)
; 7th line (TYPE=USER,
HTYPE=TORSION)
; IMETHOD,ALPHA
; 8th line (TYPE=USER,
HTYPE=PMM, USECALC=TRUE)
; IMETHOD,
ALPHA, PMAX, bSYMMETRIC
; 8th line (TYPE=USER,
HTYPE=PMM, bUSECALC=FALSE)
; R01C1,
R01C2, R01C3(, R01C4, R01C5)
; 9th line (TYPE=USER,
HTYPE=PMM, bUSECALC=FALSE)
; ...
;
...
; R11C1,
R11C2, R11C3 (, R11C4, R11C5)
; 19th line (TYPE=USER,
HTYPE=PMM, bUSECALC=FALSE) |
|
1. In the case of AXIAL, MOMENT, SHEAR,
PMM
NAME: name
of plastic hinge
TYPE: type
of plastic hinge
2. In the case of USER
NAME: name
of plastic hinge
TYPE: type
of plastic hinge {USER}
HTYPE:
user-defined type of plastic hinge
bSYMMETRIC:
whether the hinge properties are symmetrical
B, C, D, E: input
location of plastic hinge data
P: Positive
N: Negative
IO: Immediate
Occupancy
LS:
Life Safety
CP: Collapse
Prevention
YF: Yield
Force
YD:
Yield Displacement
YM: Yield
Moments
YR: Yield
Rotation
YT: Yield
Torsion
IMETHOD: apply
the Bresler Interpolation method to the P-M interaction diagrams
ALPHA:
=
1 : linear
=
2 : elliptic
bUSECALC: whether
to automatically calculate the input value of the section data |
|
*HINGE-ASSIGN (Assign
Pushover Hinges) |
|
Assigning defined hinge properties to each
element |
|
; ELEM_LIST, HINGE_TYPE,
LOCATION |
|
ELEM_LIST: element
number
HINGE_TYPE: type
of assigned hinge
LOCATION: location
of the hinge in the element |
|
*INITIAL-LOAD
(Initial Load) |
|
Initial load assigned before executing
pushover analysis |
|
; LCNAME1, FACT1, LCNAME2,
FACT2, ? :
from line |
|
LCNAME1 : unit
load condition
FACT1 : load
modulus |
|
*POLDCASE
(Pushover Load Cases) |
|
Assigning load conditions for pushover
analysis |
|
NAME=NAME, DESC ;
1st line
; CTRL_OPT,
DISPL ;
2nd line
(CTRL_OPT=GLOBAL)
; CTRL_OPT,
MNODE, DIR, DISPL ;
2nd line
(CTRL_OPT=MNODE)
; ANAL_OPT,
bUSEINILOAD, LOAD_PATTERN
;
3rd line
; DIR,
SCALE ;
4th line
(LOAD_PATTERN=UNIFORM)
; MODE,
SCALE ;
4th line
(LOAD_PATTERN=MODE)
; LCNAME1,
SCALE1, LCNAME2, SCALE2, ...
;
from 4th line (LOAD_PATTERN=STATIC) |
|
NAME: name
of unit load condition
DESC: brief
description
CTRL_OPT: assigning
method of the target displacement
1. In the case when the Control Option
is GLOBAL
DISPL: max
moving displacement
2. In the case when the Control Option
is MNODE
MNODE:
number for the main node
DIR: direction
of the moving displacement
DISPL: max
moving displacement
ANAL_OPT: conditon
of pushover analysis
bUSEINILOAD:
assigning method of the initial load
LOAD_PATTERN: assign
load type (size ratio)
1. In the case when the Load Pattern is
UNIFORM
DIR: direction
of the load
SCALE:
scale factor
2. In the case when the Load Pattern is
MODE
MODE: natural
frequency mode
SCALE:
scale factor
3. In the case when the Load Pattern is
STATIC
LCNAME1: name
of the unit load
SCALE1: scale
factor |
|
PUSHOVER-CTRL
(Pushover Analysis Control Data ) |
|
Assign the analysis conditons for pushover
analysis |
|
; iMAXINUM, iMAXITER,
TOL |
|
iMAXINUM: number
of steps to the target displacement
iMAXITER: max
iteration
TOL: convergence
tolerance |
|
ADDITIONAL-STEP (Additional
Steps for Pushover Analysis) |
|
Assign the location of a specific step
where the user wishes to check
the results |
|
; STEP1, RATIO1, STEP2,
RATIO2, ... ;
from line 1 |
|
STEP1: initial
step required to determine the location of the additional step
RATIO1: distance
ratio from the initial step |
|
*LOAD-SEQ (Loading
Sequence) |
|
Assigning the order of applying loads in
a
geometrical nonlinear analysis |
|
; LCNAME1, LCNAME2, ...
;
from line 1 |
|
LCNAME1: Static
Load Cases in the order of application |
|
*STAGE
(Define Construction Stage ) |
|
Defining construction stages to carry out
the
construction stage analysis of a bridge
* Where PSC box bridges are analyzed: Wizards,
which
automatically define the construction stages,
are
provided for different construction methods
such as
ILM,FCM, MSS, etc. |
|
; NAME=NAME, DURATION,
bSAVESTAGE
bSAVESTEP ;
line 1
; STEP=DAY1, DAY2, ...
;
line 2
; AELEM=GROUP1, AGE1,
GROUP2, AGE2, ... ;
line 3
; DELEM=GROUP1, REDIST1,
GROUP2, REDIST2, ...
;
line 4
; ABNDR=BGROUP1, POS1,
BGROUP2, POS2, ... ;
line 5
; DBNDR=BGROUP1, BGROUP2,
... ;
line 6
; ALOAD=LGROUP1, DAY1,
LGROUP2, DAY2, ... ; line 7
; DLOAD=LGROUP1, DAY1,
LGROUP2, DAY2, ... ; line 8 |
|
NAME: name
of the construction stage
DURATION: duration
of the construction stage
bSAVESTAGE: analysis
results are saved by constrution stages
bSAVESTEP: analysis results are saved by
Steps within a construction stage
STEP: elapsed
time to be defined as Step within the duration of the
construction stage
AELEM: activation
of element groups to define active elements
within a corresponding
construction stage
= GROUP1: defining active
element groups
= AGE1:
member age of the group
DELEM: inactivation
of element groups
= GROUP1: defining inactive
element groups
= REDIST1: Element Force
Reduction, which the percentage of
the internal forces carried
by the elements to be deactivated will be
redistributed to the contigous
elements
ABNDR: activation of boundary groups to
define active boundart
conditions within a corresponding construction
stage
= BGROUP1: defining active boundary condition
groups
= POS1: determining the right positions
where a boundary
condition contains restraint conditions
or elastic support conditions
= DEFORMED: applying the boundary conditions
at the locations
after the strucure has deformed
= ORIGINAL: applying the boundary conditions
at the original
locations of the strucural nodes
DBNDR: inactivation
of boundary group conditions
= BGROUP1: boundary conditon
groups to be deactivated
ALOAD: activation
of load groups to define active load cases
within a corresponding
construction stage
= LGROUP1: load groups
to be activated
= DAY1: time for activating
load groups
DLOAD: inactivation
of load groups
= LGROUP1: load groups to be deactivated |
|
*LOADCOMB (Combinations
) |
|
Load combination conditions to combine
the results
of static analysis, moving load analysis,
response
spectrum
analysis, time dependent analysis, etc. |
|
; NAME=NAME, KIND, iTYPE,
DESC ;
line 1
; ANAL1, LCNAME1, FACT1,
... ;
from line 2 |
|
NAME: name
of load combination condition
= gLCB: General LCB
= cLCB: Concrete LCB
= sLCB: Steel LCB
= rLCB: SRC LCB
= fLCB:
Footing LCB
KIND: type
of load combination
= GEN: General= STEEL:
Steel Design
= CONC: Concrete Design
= SRC: SRC Design
= FDN: Footing Design
iTYPE: type
of load combination method {0}
= 0 : Linear
= 1 : +SRSS
= 2 : -SRSS
DESC: brief
ciscription
ANAL1: type
of load case
= ST: Static
= RS: Response Spectrum
= TH: Time History
= MV: Moving
= SM: Settlement
LCNAME1: names
of load cases
FACT1: load
factors to be applied to load cases {1} |
|
*ANAL-CTRL |
|
Number of maximum iterations and
convergence tolerance when analysis is
performed using nonlinear elements and
the
basic boundary conditions of individual
elements in a structure |
|
bARDC:
auto rotational DOF constratint for truss/plane stress/solid elements(YES/NO)
bANRC:auto
normal rotation constraint for plate elements(YES/NO)
iTYPE: type
of analysis method when performing an analysis using nonlinear elements
= 0 : when performing
a repetetive analysis, stiffness of inactive members is included.
= 1
: when performing a repetetive analysis, stiffness of inactive members
is excluded.
iITER: maximum
number of iterations when performing an
analysis using nonlinear
elements
TOL: convergence
tolerance when performing an analysis using nonlinear elements
iSITER:
number of iterations for which loads are used to check the convergence
condition in each repetitive analysis
stemming from changing stiffness of
the structure for each
load case |
|
*PDEL-CTRL (P-Delta
Analysis Control ) |
|
Load cases and control for iteration required
for
carrying out buckling analysis of a structure |
|
; iITER, TOL ;
line 1
; LCNAME1, FACT1, LCNAME2,
FACT2, ... ;
from line 2 |
|
iITER:
number of iterations for P-Delta analysis {5}
TOL: convergence
tolerance{1e-5}
LCNAME1: name
of load case
FACT1: load
factor {1} |
|
*BUCK-CTRL (Buckling
Analysis Control) |
|
Load cases and related data required for
carrying
out buckling analysis of a structure |
|
; iMODENUM, iITER, TOL
;
line 1
; LCNAME1, FACT1, LCNAME2,
FACT2, ... ;
from line 2 |
|
iMODENUM: number
of buckling modes {0}
iITER: number
of iterations required for the process of Subspace
Iteration in a buckling
analysis {30}
TOL: convergence
tolerance{1e-6}
LCNAME1: casename
of load
FACT1: load
factor {1} |
|
*EIGEN-CTRL
(Eigenvalue Analysis Control ) |
|
Control data for eigenvalue analysis |
|
iFREQ: requencinumber
of natural fes for the structure {0}
iITER: number
of iterations required for eigenvalue analysis {20
}iDIM: size
of Subspace {0}
TOL: convergence
tolerance {1e-6}
bINCNI: include
NL-link force vectors(YES/NO) {NO}
iGNUM: number
of generations for each NL-link force vectors |
|
*SPEC-CTRL
(Response Spectrum Analysis Control) |
|
Combination method of modes in a response
spectrum analysis |
|
; TYPE, DAMPING, bADDSIGN |
|
TYPE:
method of combining modes in a response spectrum analysis
= SRSS, CQC, ABS {SRSS}
DAMPING: damping
ratio
bADDSIGN:
whether to revive signs in the analysis results
= YES: use of (+), (-)
when combining modes
= NO: do not use signs |
|
*MOVE-CTRL
(Moving Load Analysis Control) |
|
Analysis method and output locations of
element
results in a moving load analysis |
|
; METHOD, POINT, PLATE,
, FRAME,
,.bREAC, bRG, RGN, bDISP,
bDG, DGN, bFM, bFG, FGN |
|
METHOD: method
of moving load analysis {1}
= 1 : Exact
= 2 : Pivot
= 3 : Quick
POINT: point
of vehicle load application
PLATE: calculation
of member forces of plate elements per unit length {1}
= CENTER: calculation
of member force per unit length relative to
the center point of the
element
= NODAL: calculation of
member force per unit length relative to
the center point of the
element and the nodes composing the element
Frame:
member force output at 5 Points for Frame elements
=NORMAL:
member forces at 5 Points for beam elements
=Axial: calculating the
member forces at 5 Points, max/min axial
force and moments are
calculated and produced
bREAC: option
to output the reaction values when producing the
output for moving load
analysis results for a reaction (YES/NO) {YES}
bRG: option
to assign groups when producing output for reaction values (YES/NO) {NO}
RGN: name
of the assigned group when producing output for reaction values
bDISP:
option to output the displacement values when producing
the output for moving
load analysis results for a displacement
(YES/NO) {YES}
bDG: option
to assign groups when producing output for
displacement values (YES/NO)
{NO}
DGN: name
of the assigned group when producing output for
displacement values
bFM: option
to output the member force values when producing the
output
for moving load analysis results for a member force (YES/NO) {YES}
bFG: option
to assign groups when producing output for
member force values (YES/NO)
{NO}
FGN: name
of the assigned group when producing output for
member force values |
|
*HYD-CTRL
(Hydration Analysis Control ) |
|
Aalysis conditions required for heat of
hydration analysis |
|
; bLAST-FINAL, STAGE,
CN-FACTOR, INIT-TEMPER, EVALUATION, bCNS, TYPE, iITER, TOL |
|
bLAST-FINAL: selection
of a construction stage, which is
considered as the Final
stage of the structure during the
construction-staged heat
of hydration analysis
= YES: Last Stage
= NO: Other Stage
STAGE: construction
stage to be applied as the final stage
CN-FACTOR: Temporal
Discretization Factor in heat transfer analysis
INIT-TEMPER: initial
temperature used in heat transfer analysis
EVALUATION: location
of a solid element for which stresses are produced
= CENTER: stess in the
center point of the solid element used as the stess in the
entire element
= GAUSS: Gauss integration
point stresses used as the nodal stresses
= NODAL:
interpolated nodal stresses using the Gauss integration point stresses
bCNS: option
to reflect the effects or creep and shrinkage
(YES/NO) {NO}
TYPE: select
ion of creep and shrinkage
= CREEP: consider only
creep
= SHRINK: consider only
shrinkage
= BOTH: consider both
creep and shrinkage
iITER:
max number of iterations for an analysis reflecting creep
TOL: convergence
tolerance |
|
*NONL-CTRL (Nonlinear
Analysis Control ) |
|
Assignment of analysis conditions required
for a
nonlinear analysis considering large displacements |
|
; ITER, LSTEP, MAX, bENGR,
EV, bDISP, DV, bFORC, FV
;
ITER=NEWTON
; ITER, IFR, MINC, MITER,
MDISP bENGR, EV, bDISP, DV,
bFORC, FV ;
ITER=ARC |
|
1. In the case of Newton-Raphson
ITER: selection
of the method of iterative analysis
= NEWTON: Newton-Raphson
= ARC: Arc-Length
LSTEP: total
load divided into the number of Load Steps and applied to each step.
MAX: maximum
number of iterations of analysis for each Load Step
bENGR: assement
of convergence by Norm base value of energy
(load ¢¥displacement) (YES/NO)
{NO}
EV: energy
Norm
bDISP: assement
of convergence by Norm base value of
displacement (YES/NO) {NO}
DV: displacement
Norm
bFORC: assement
of convergence by Norm base value of
member force
(YES/NO)
{NO}
FV: member force Norm
2. In the case of Arc-Length
IFR:
Ratio of the Initial Force for Unit Arc-Length
MINC: maximum
number of increment steps
MITER: maximum
number of iterations of analysis for each Increment Step
MDISP: magnitude
of maximum displacement |
|
*STAGE-CTRL (Construction
Stage Analysis Control Data ) |
|
Assignment of analysis conditions required
for using
the analysis functions for a bridge by
construction stages |
|
; bLAST-FINAL, FINAL-STAGE,
;
line 1
; bINC-NLA, iMAXITER,
bENEG, EV, bDISP, DV, bFORC,
FV ;
line 2
; bINC-TDE, bCNS, TYPE,
iITER, TOL,
;
line 3
; bOUCC, bITS, iITS, bATS,
iT10, iT100, iT1K, iT5K, iT10K
;
line 4 |
|
bLAST-FINAL: selection
of a construction stage, which is considered
as the Final stage of
the structure during the construction stage analysis
= YES: Last Stage
= NO: Other Stage
FINAL-STAGE: construction
stage to be applied as the final stage
bINC-NLA: option
to include nonlinear analysis reflecting the
change
of geometric shapes (YES/NO) {NO}
iMAXITER: max
number of iterative analyses for each Load Step
bENEG: assement
of convergence by Norm base value of
energy (load ¢¥displacement)
(YES/NO)
{NO}
EV: energy
Norm
bDISP:
assement of convergence by Norm base value of
displacement
(YES/NO) {NO}
DV: displacement
Norm
bFORC: assement
of convergence by Norm base value of
member
force (YES/NO) {NO}
FV: member
force Norm
bINC-TDE: option
to analyze the structure by reflecting the time
dependent material properties
(YES/NO) {NO}
bCNS: option
to consider creep and shrinkage (YES/NO) {NO}
TYPE: select
ion of creep and shrinkage
= CREEP: consider only
creep
= SHRINK: consider only
shrinkage
= BOTH: consider both
creep and shrinkage
iITER:
max number of iterations when performing an analysis reflecting creep
TOL: convergence
tolerance
: option
to consider creep and shrinkage when
reflecting
the tension force loss in tendons (YES/NO) {NO}
: option
to apply the change of modulus of elasticity of
concrete
based on member ages (YES/NO) {NO}
: option
to consider elastic shortening when reflecting
the tension force loss
in tendons (YES/NO) {NO}
bOUCC:
only the user-specified creep coefficient used (YES/NO) {NO}
bITS: option
to create Additional Step when considering creep (YES/NO)
iITS: number
of Time Steps to be created internally
bATS: option
to automatically create Time step when T (Time Gap) is large (YES/NO)
iT10:
number of Time steps to be created when T>10
iT100: number
of Time steps to be created when T>100
iT1K: number
of Time steps to be created when T>1000
iT5K: number
of Time steps to be created when T>5000iT10K: number of Time steps
to be created
when T>10000 |
|
*DGN-MATL (Modify
Steel (Concrete) Material) |
|
Used when changing input material data
or when
modifying the material data of concrete
and steel |
|
; iMAT, TYPE, MNAME, [DATA1]
;
STEEL
; iMAT, TYPE, MNAME, [DATA2],
RBCODE, RBMAIN
RBSUB, FCI ; CONC
; iMAT, TYPE, MNAME, [DATA3],
[DATA4], RBCODE
RBMAIN ;
SRC
; [DATA1] : 1, DB, NAME
or 2, ELAST, POISN, DEN, FU,
FY1, FY2, FY3, FY4
; [DATA2] : 1, DB, NAME
or 2, ELAST, POISN, DEN, FC
; [DATA3] : 1, DB, NAME
or 2, ELAST, FU, FY1, FY2, FY3, FY4
; [DATA4] : 1, DB, NAME
or 2, ELAST, FC |
|
iMAT:
material number
TYPE: type
of material
= CONC
= STEEL
= SRC
MNAME: name
of material
RBCODE: select
a standard for reinforcing steel
=
KS (RC)
= KS-Civil (RC)
RBMAIN: material
of the main reinforcing steel
= SD 24
= SD 30
= SD35
= SD40
RBSUB:
material of the beam reinforcing steel (shear steel)
= SD 24
= SD 30
= SD35
= SD40
In the case of [DATA1]
1 = DB: Database
(*refer to MATERIAL)
NAME: name
of the database
2 = ELAST: modulus
of elasticity
POISN:
poisson’s ratio
DEN: density
FU: Tensile
Strength
FY1~FY4: Yield
strenths for different thicknesses of members
based on applicable standard
In the case of [DATA2]
2 = ELAST: elastic
modulus of concrete
POISN: poisson’s
ratio of concrete
DEN: density
of concrete
FC: design
standard strength of concrete |
|
*DGN-SECT |
|
Printing out forces of plate elements in
a graph form at a selected cutting line |
|
; iSEC, TYPE, SNAME, OFFSET,
SHAPE, [DATA]
{, CCSHAPE} ;
DB/USER
; iSEC, TYPE, SNAME, OFFSET,
SHAPE, BLT, D1, D2, D3,
D4, D5, D6 ;
1st line - VALUE
; AREA,
ASy, ASz, Ixx, Iyy, Izz ;
2nd line
; CyP,
CyM, CzP, CzM, QyB, QzB, PERI_OUT, PERI_IN
Cy, Cz ;
3rd line
; iSEC, TYPE, SNAME, OFFSET,
SHAPE, iREPLACE
ELAST, DEN, POIS, POIC
;
1st line - SRC
; D1,
D2, [DATA] ;
2nd line
; iSEC, TYPE, SNAME, OFFSET,
SHAPE, 1, DB, NAME1,
NAME2, D1, D2 ;
COMBINED
; iSEC, TYPE, SNAME, OFFSET,
SHAPE, 2, D11, D12, D13,
D14, D15, D21, D22, D23,
D24
; iSEC, TYPE, SNAME, OFFSET,
SHAPE, iyVAR, izVAR
STYPE ;
1st line - TAPERED
; DB,
NAME1, NAME2 ;
2nd line (STYPE=DB)
; [DIM1],
[DIM2] ;
2nd line (STYPE=USER)
; D11,
D12, D13, D14, D15, D16 ;
2nd
line (STYPE=VALUE)
; AREA1,
ASy1, ASz1, Ixx1, Iyy1,
Izz1 ;
3rd line (STYPE=VALUE)
; CyP1,
CyM1, CzP1, CzM1, QyB1, QzB1, PERI_OUT1
PERI_IN1, Cy1, Cz1 ;
4th line(STYPE=VALUE)
; D21,
D22, D23, D24, D25, D26 ;
5th
line (STYPE=VALUE)
; AREA2,
ASy2, ASz2, Ixx2, Iyy2,
Izz2 ;
6th line (STYPE=VALUE)
; CyP2,
CyM2, CzP2, CzM2, QyB2, QzB2, PERI_OUT2,
PERI_IN2, Cy2, Cz2 ;
7th line (STYPE=VALUE)
; [DATA] : 1, DB, NAME
or 2, D1, D2, D3, D4, D5, D6
; [DIM1], [DIM2] : D1,
D2, D3, D4, D5, D6 |
|
* refer
to Section |
|
*DGN-CTRL (General
Design Data) |
|
Input required data for design |
|
; bFRAMEX, bFRAMEY, bAUTOKF
;
1st line
; STORY1, XMIN1, XMAX1,
YMIN1, YMAX1, RMIN1,
RMAX1 ;
2nd line
; ... ;
...
; STORYn, XMINn, XMAXn,
YMINn, YMAXn, RMINn
RMAXn ;
n+1th line |
|
bFRAMEX: define
Unbraced | Sway or Braced | Non-sway frame in the global X-direction.
bFRAMEY: define
Unbraced | Sway or Braced | Non-sway frame in the global Y-direction.
bAUTOKF: select
if the effective buckling length factors are to be automatically calculate.d
LC1: the
live load cases that the live load reduction factor is applicable
RT:
the methods for calculating the live reduction factor
0
= General Design Code
1
= Chinese Standard
DT: design
type
3D: 3-D
XY:
X-Y plane
XZ: X-Z
plane
YZ:
Y-Z plane
bAF: live
load reduction factor of axial force(YES/NO)
bMO: live
load reduction factor of moments(YES/NO)
bSF:
live load reduction factor of shear force(YES/NO)
STORY1: name
of the reference story where the live load reduction factor is to be applied
XMIN1, XMAX1:
the minimum(maximum) global X-coordinate
YMIN1, YMAX1: the
minimum(maximum) global Y-coordinate
RMIN1, RMAX1:
The range within which the live load reduction factor is to be applied |
|
*DGN-STEEL
(Steel Design Code) |
|
Select the design code to apply for the
strength verification of steel members and specify
the lateral bracing condition of the structure's
horizontal members (beams and girders |
|
; CODE, bBRACED, bSPSEIS,
iCLASS |
|
CODE: Steel
design code { AISC-LRFD93 }
= AISC-LRFD 2k & 93
= AISC-ASD89
= BS5950-90
= Eurocode3
= CSA-S16-01
= AISI-CFSD86
bBRACED: Specify
the lateral brace condition to the horizontal members (beams and girders)
of the
structure
to be designed (YES/NO){NO}
bSPSEIS: whether
to apply the Special Provisions for Seismic Design according to GBJ17-88
Code
iCLASS: earthquake
resistance grade when the Special Provisions for Seismic Design according
to
GBJ17-88
Code
= 0: Grade -1
= 1: Grade-2
= 2: Grade-3
= 3: Grade-4
safety grade of the structure
when not applied
= 0: Level 1 (Strategic)
= 1: Level 2 (Primary)
= 2: Level 3 (Secondary) |
|
*DGN-CONC
(Concrete Design Code) |
|
Determine the applicable design code and
the applicability of special provisions for seismic
design for the design of or the strength
verification for RC members |
|
; CODE, bSPECIAL, PHI-B,
PHI-T, PHI-C1, PHI-C2, PHI-V,
RHOW, RHOC, RHOR, KIND
;
line 1
; TLF, SLF ;
line 2
; COMB1, COMB2, COMB3,
... |
|
CODE: RC
design code { ACI318-02 }
= ACI318-02/99/95/89
= CSA-A23.3-94
= BS8110-97
= Eurocode2
bSPECIAL: Option
to apply the special provisions for seismic design (YES/NO){NO}
PHI-B: Strength
reduction factor for pure flexure or flexure + axial tension {0.85}
PHI-T:
Strength reduction factor for axial tension {0.85}
PHI-C1: Strength
reduction factor for spirally reinforced columns subjected
to axial compression or
flexure + axial compression {0.75}
PHI-C2: Strength
reduction factor for tied columns subjected to axial compression or flexure
+ axial
compression
{0.7}
PHI-V: Strength
reduction factor for shear {0.8}
RHOW: Limiting
maximum rebar ratio for shear wall members {0.04}
RHOC: Limiting
maximum rebar ratio for column members {0.03}
RHOR: Limiting
maximum rebar ratio for brace members {0.03}
KIND: design
methods for Column and Brace according to AIJ-WSD99 Code
0 = method 1 (by N+My,
N+Mz)
1 = method 2 (by fixed
N, combined My, Mz)
2 = method 3 (by rotated
Neutral Axis) |
|
*DGN-SRC
(SRC Design Code) |
|
Enter the design code applicable for strength
verification of SRC
(Steel-Reinforced Concrete composite) members |
|
; CODE, iMATERIAL, bSPSEIC,
iCLASS |
|
CODE: SRC
design code {SSRC79}
IMATERIAL:
material type
= 0 : SRC
bSPSEIC: whether
to apply the Special Provisions for Seismic Design according to JGJ138-01
Code
iCLASS: whether
to apply the Special Provisions for Seismic Design according to JGJ138-01
Code
= 0: Grade-1
= 1: Grade-2
= 2: Grade-3
= 3: Grade-4
safety grade of the structure
when not applied
= 0: Level 1 (Strategic)
= 1: Level 2 (Primary)
= 2: Level 3 (Secondary) |
|
*CB-FACTOR (Bending
Coefficient) |
|
Bending Coefficient required for calculating
the allowable bending stress or the design
strength of the compression flange subjected
to the bending moment about the strong axis (y-axis) |
|
; ELEM_LIST, bAUTOCALC,
CB |
|
ELEM_LIST: element
number
bAUTOCALC: apply
this item if the value is to be auto-calculated by the program (YES/NO){NO}
CB: bending
coefficient {1} |
|
*CM-FACTOR (Moment
Factor) |
|
the Equivalent Moment correction Factor
of the beam-column members |
|
; ELEM_LIST, bAUTOCALC,
CMy, CMz |
|
ELEM_LIST: element
number
bAUTOCALC: apply
this item if the value is to be auto-calculated by the program
(YES/NO){NO}
CMy:
Equivalent moment correction factor applied to the unbraced length portion
of a member bent
about
its strong axis {0}
CMz:
Equivalent moment correction factor applied to the unbraced length portion
of a member bent
about
its weak axis {0} |
|
*CV-FACTOR (Shear
Coefficient) |
|
Shear coefficient |
|
; ELEM_LIST, bAUTOCALC,
CV |
|
ELEM_LIST: element
number
bAUTOCALC: apply
this item if the value is to be auto-calculated by the program (YES/NO){NO}
CV: shear
coefficient |
|
*DFN-ALLOWABLE (SpecifyAllowable
Stress) |
|
Enter the allowable stress coefficients
if user may wish to define the
allowable stresses |
|
; ELEM_LIST, FA, FT, FBy,
FBz, FV |
|
ELEM_LIST : element
number
FA: Allowable
compression stress coefficient for the compressive force along the member's
axial
direction
{0.5}
FT:
Allowable tension stress coefficient for the tensile force along the member's
axial direction {0.6}
FBy: Allowable
bending stress coefficient for the bending moment about the member's strong
axis {0.6}
FBz: Allowable
bending stress coefficient for the bending moment about the member's weak
axis {0.6}
FV: Allowable
shear stress coefficient for the shear force {0.4} |
|
*F-MAGNIFY
(Moment Magnifier) |
|
Moment Magnification Factors |
|
; ELEM_LIST, B1y, B1z,
B2y, B2z |
|
ELEM_LIST
: element number
B1y:
Moment magnification factor for members subjected to vertical loads in
a frame braced against
sidesway for strong axis
bending {0}
B1z:
Moment magnification factor for members subjected to vertical loads in
a frame braced against
sidesway
for weak axis bending {0}
B2y: Moment
magnification factor for members subjected to horizontal loads in a frame
unbraced
against
sidesway for strong axis bending {1}
B2z: : Moment
magnification factor for members subjected to horizontal loads in a frame
unbraced
against
sidesway for weak axis bending. {1} |
|
*K-FACTOR (Effective
Length Factor) |
|
Effective Length Factors for the unbraced
lengths |
|
; ELEM_LIST, Ky, Kz |
|
ELEM_LIST: element
number
Ky:
Effective buckling length factor for buckling about strong axis {1}
Kz: Effective
buckling length factor for buckling about weak axis {1} |
|
*LENGTH (Unbraced
Length) |
|
the unbraced lengths for buckling about
the strong (y-axis) and weak (z-axis) axes of the
selected compression membersthe laterally
unbraced length for the compression flange of a
member bent about its weak axis |
|
; ELEM_LIST, Ly, Lz, bNOTUSE,
Lb, bAUTOCALC, Le |
|
ELEM_LIST :
element number
Ly: Unbraced
length for buckling about strong axis (determined by braces in z-dir.)
Lz:
Unbraced length for buckling about weak axis (determined by braces in
y-dir.)
bNOTUSE: Select
this item, if the allowable bending stress computation about the member`s
strong axis
is to
neglect the laterally unbraced length (YES/NO){NO}
Lb: Laterally
unbraced length
bAUTOCALC: Select
this item, if the Effective Unbraced Length, Le is auto-calculated according
to the BS
5950-90
Code
Le: the
Effective Unbracedl Lngth according to the BS 5950-90 Code |
|
*REDUCTION
( Modify Live Load Reduction Factor) |
|
Reduction factor of the live loads acting
on the relevant columns, shear
walls or footings when calculating the
required axial strength |
|
; ELEM_LIST, FACTOR |
|
ELEM_LIST:
element number
FACTOR:
Live load reduction factor {1} |
|
*MEMBERTYPE (ModifyMember
Type) |
|
The type of members used in the design
of steel and RC members |
|
; ELEM_LIST, TYPE |
|
ELEM_LIST: element
number
TYPE: the
member type to be used in design
= Beam
= Column
= Brace |
|
*STIFFENER (Longitudinal
Stiffener of Box Section) |
|
The spacings and size of transversal/longitudinal
stiffeners for box sections |
|
; iSEC, ASTF, BSTF, TSTF,
iNOy, iNOz |
|
iSEC:
Section property number for the box member for which the strength is be
verified
ASTF:
Spacing of the transverse stiffeners
BSTF:
Width of the longitudinal stiffener
TSTF:
Thickness of the longitudinal stiffener
iNOy:
Number of panels on the flange side separated by the longitudinal stiffeners
{2}
iNOz:
Number of panels on the web side separated by the longitudinal stiffeners
{2} |
|
*LIMITSRATIO (Limit
Slenderness Ratio ) |
|
Allowable limit slenderness ratio |
|
; ELEM_LIST, bNOTCHECK,
COMP, TENS |
|
ELEM_LIST: element
number
NOTCHECK: Select
this item if the limiting slenderness ratios (KL/r)
are of no interest. If
selected, design results reflecting the slenderness effects are
not produced. (YES/NO){NO}
COMP: Limiting
slenderness ratio for members under axial compression {200}
TENS:
Limiting slenderness ratio for members under axial tension {300} |
|
*DGNCRITERIA (Design
Criteria of Rebar) |
|
Enter the standard sizes of main and sub-rebars
used in the design of beam, column and
brace members.Also, enter the standard
sizes and spacing for vertical and horizontal
rebars used in the design of shear wall
members. |
|
; STIR, SIDE, DT, DB,
MAIN1, MAIN2, MAIN3, MAIN4
MAIN5, iSRBN ;
line 1 - beam
; STIR, DO, MAIN1, MAIN2,
MAIN3, MAIN4, MAIN5
iSRBN ;
line 2 - column
; STIR, DO, MAIN1, MAIN2,
MAIN3, MAIN4, MAIN5
iSRBN ;
line 3 - brace
; END, HORZ, DE, DW, VERT1,
VERT2, VERT3, VERT4,
VERT5 ;
line 4 - wall
; DIST1, DIST2, DIST3,
iMETHOD, bBEND
;
line 5 - spacing1
; HORZ, VERT1, VERT2,
VERT3, ..., VERT50
;
line 6 - spacing2 |
|
1. For
Beam Design
STIR: Standard
sizes for transverse reinforcing bars in beam design {D10}
SIDE: Standard
sizes for side bars, used for bar placing. Beam strength is not affected
{D13}
DT: Distance
between the center of the main rebars in the top layer of the top bars
and the top surface
of the
section {0}
DB: Distance
between the center of the main rebars in the lower layer of the bottom
bars and the
bottom
surface of the section {0}
MAIN1: Main
rebar standard sizes for the design of beam members {D22}
iSRBN: Number
of shear reinforcement legs
2. For Column Design
STIR: Standard
sizes for tie bars used in column design {D10}
DO: Distance
between the center of the main rebars and the perimeter surface of the
section {0}
MAIN1: Main
rebar standard sizes for the design of column members {D22}
iSRBN: the
number of layers in the stirrup rebars
3. For Brace Design
STIR: Standard
sizes for tie bars used in brace design {D10}
DO: Distance
between the center of the main rebars and the perimeter surface of the
section {0}
MAIN1: Main
rebar standard sizes for the design of brace members {D22}
* If d0 is not entered
(ie. 0), the program uses the larger of 2.5?(63.5mm) and H/10, but not
exceeding
3 inches
4. For Shear Wall Design
END: The
minimum standard size to be used for end rebars for shear wall design
{D10}
HORZ: Standard
size for horizontal rebars used in shear wall design {D10}
DE: Distance
from the end of the shear wall member to the center of the first row of
the vertical rebars
(or
end rebars) {0}
DW: Distance
between the center of the end vertical rebars and the end of the shear
wall {0}
VERT1:
Standard sizes for vertical rebars used in shear wall design {D13}
Spacing1
DIST1: Spacing
of end rebars in the case of 4 end rebars {0.3M}
DIST2: Spacing
of end rebars in the case of 6 end rebars {0.15M}
DIST3:
Spacing of end rebars in the case of 8 end rebars {0.1M}
iMETHOD: The
method of designing shear walls considering end rebars {1}
= 1: Method-1
= 2: Method-2
= 3: Method-3
= 4: Method-4
bBEND: Determine
whether to design the wall for a bending moment about the weak axis (YES/NO){NO}
Spacing2
HORZ: Spacing
of horizonal rebars {0}
VERT1: Spacing
of vertical rebars {0}
* If the values dw and
de are not entered (in case where they are 0), 2 inches (5.08cm) are
automatically used. |
|
*REBAR-BEAM (Modify
Beam Section Data) |
|
Enter the section dimensions and rebar
data for RC beam members for strength verification |
|
; iSEC, SBARNAME, DT,
DB ;
line1
; iTIARR, iTIRB1, iTIRB2,
TINAME, iBIARR, iBIRB1
iBIRB2, BINAME, ISPACE,
iISRBN ;
line 2
; iTMARR, iTMRB1, iTMRB2,
TMNAME, iBMARR,
iBMRB1, iBMRB2, BMNAME,
MSPACE, iMSRBN ;
line 3
; iTJARR, iTJRB1, iTJRB2,
TJNAME, iBJARR, iBJRB1,
iBJRB2, BJNAME, JSPACE,
iJSRBN ;
line 4 |
|
iSEC: property
number of the beam members
SBARNAME :
Standard sizes of the stirrup rebar
DT: Distance
between the center of the top main rebars in the upper layer and the top
surface of the
section
{0}
DB: Distance
between the center of the bottom main rebars in the lower layer and the
bottom surface of
the
section {0}
iTIARR:
Top rebar data at node i of the beam members {1}
= 1: one layer
= 2: two layers
iTIARB1: Number
of top rebars in the upper layer at node i
iTIARB2: Number
of top rebars in the lower layer at node i
TINAME:
Standard sizes of the top rebar
iBIARR: Bottom
rebar data at node i of the beam members {1}
= 1: one layer
= 2: two layers
iBIRB1: Number
of bottom rebars in the upper layer at node i
iBIRB2:
Number of bottom rebars in the lower layer at node i
BINAME: Standard
sizes of the bottom rebar
ISPACE: Spacing
of stirrup bars
iISRBN: the
number of layers of the stirrup rebars in the i node section
* line3 and line4 each
shows the rebar information of the Middle,
J end. The
form is the same as line2,
so therefore omitted
* when using the initial
value ??as the cover thickness, the value automatically calculated within
the program will be used in the element design and strength inspection |
|
*REBAR-COLUMN
(Modify Column Section Data) |
|
Enter the section dimensions and rebar
data for RC column members for strength
verification. |
|
; iSEC, HOOP, RBNAME,
iNQRB, iNROW, DO, SRBNAME, SPACE, iSRBN |
|
iSEC: property
number of the column members
HOOP :
the type of hoop rebars {Tied}
= TIED
= SPIRAL
RBNAME: Standard
sizes of the main rebar
iNQRB:
Number of vertical rebars placed in the column section
iNROW: Number
of rows of vertical rebars placed in the column section
DO:
Distance between the center of the main rebars and the perimeter surface
of the section {0}
SRBNAME:
Standard sizes of the hoop rebar
SPACE: Spacing
of hoop rebars
iSRBN: the
number of layers in the stirrup rebars in the arrangement section
* when using the initial
value ??as the cover thickness, the value automatically calculated within
the program will be used in the element design and strength inspection. |
|
*REBAR-BRACE (Modify
Brace Section Data) |
|
Enter the section dimensions and rebar
data for RC brace members for strength verification |
|
; iSEC, HOOP, RBNAME,
iNQRB, iNROW, DO, SRBNAME, SPACE, iSRBN |
|
iSEC: property
number of the brace members
HOOP: the
type of hoop rebars {Tied}
= TIED
= SPIRAL
RBNAME: Standard
sizes of the main rebar
iNQRB:
Number of vertical rebars placed in the brace section
iNROW: Number
of rows of vertical rebars placed in the brace section
DO: Distance
between the center of the main rebars and the surface of the section {0}
SRBNAME: Standard
sizes of the hoop rebar
SPACE: Spacing
of hoop rebars
ISRBN: the
number of layers in the stirrup rebars in the arrangement section
* when using the initial
value ??as the cover thickness, the value automatically calculated within
the program will be used in the element design and strength inspection. |
|
*REBAR-SRC
(Modify SRC Section Data) |
|
Enter the rebar data and SRC section data
required to perform strength verification of
Steel-Reinforced Concrete Composite Columns. |
|
; iSEC, bCALC, SPACE,
RBNAME, iNQRB, iNROW, DO, SRBNAME, SSPACE |
|
iSEC:
Section property number for which the SRC members
bCALC:
Select the option if the spacing of main rebars is to be auto-calculated
in the program. (YES/NO)
{NO}
SPACE:
spacing of the main rebars
RBNAME:
the standard size of the main rebars
iNQRB:
the number of the main rebars
iNROW:
Number of main rebar rows in the SRC section.
DO:
Distance (cover thickness) from the center of the main rebars to the face
of the concrete section {0}
SRBNAME:
Standard sizes of the stirrup rebar
SSPACE:
Spacing of stirrup rebars
* Enter the cover thickness
of the main rebars in the SRC section. If the cover thickness is not entered
for the main rebars (do = 0), the program calculates as follows :
do = MAX (Hc/10, Bc/10,
2.5) in ¡Â 3 in |
|
*REBAR-WALL (Modify
Wall Section Data) |
|
Enter the design criteria for shear wall
members- the standard rebar sizes, the rebar
placement, the number of rebars, the thickness
of the shear wall section, etc., for the
stories assigned by the user for strength
verification. |
|
; iWID, STORY, bMODELTHK,
THIK, VRBNAME, VRBSPACE, ERBNAME, ERBSPACE, iERBNUM, HRBNAME, HRBSPACE,
DW, DE |
|
iWID: Shear
wall ID number
STORY: The
story Names from which the design data are applicable
bMODELTHK: Select
the option if the thickness of the shear wall member is to be applied.
(YES/NO)
{NO}
THIK: Thickness
of the shear wall member
VRBNAME: the
standard rebar size of the vertical rebars in the shear wall member
VRBSPACE: the
spacing of the vertical rebars in the shear wall member
ERBNAME: the
standard size of the end rebars
ERBSPACE:
the spacing size of the end rebars
iERBNUM: the
number of end rebars
HRBNAME: the
standard rebar size of the horizontal rebars in the shear wall member
HRBSPACE: the
spacing of the horizontal rebars in the shear wall member
DE: Distance
from the end of the shear wall member to the center of the first row of
the vertical rebars
{0}
DW:
Distance from the center of the the end vertical rebars to the end of
the shear wall {0}
* when using the initial
value ??as the cover thickness, the value automatically calculated within
the program will be used in the element design and strength inspection |
|
*WALLMARK
(Modify Wall Mark Data) |
|
Group names or individual names for the
purpose of classification of shear walls for
automatic design or strength verification |
|
; MARKNAME, WID_LIST |
|
MARKNAME: Group
or individual name that classifies the shear wall members
WID_LIST : List
of shear wall member numbers |
|
*SUP-EQ (Scale
Up Factor for Earthquake) |
|
The scale up factor in respect to the load
combination that includes the
seismic load conditions and the seismic
load. It is applied to the Chinese standards |
|
; ELEM_LIST, LC-AXIAL,
LC-MOMENT, LC-SHEAR, LCB
AXIAL, LCB-MOMENT, LCB-SHEAR |
|
ELEM_LIST :
element number
LC-AXIAL: the
scale up factor in respect to the axial force of the
seismic
load conditions
LC-MOMENT: the
scale up factor in respect to the moment of the
seismic load conditions
LC-SHEAR: the
scale up factor in respect to the shear force of the
seismic
load conditions
LCB-AXIAL: the
scale up factor in respect to the axial force of the load
combination that includes
seismic loads
LCB-MOMENT: the
scale up factor in respect to the moment of the load
combination that includes
seismic loads
LCB-SHEAR: the
scale up factor in respect to the shear force of the load
combination that includes
seismic loads |
|
*CUTLINE
(Cutting Line) |
|
Graphic output of internal forces of plate
elements along a cutting line |
|
; NAME, DIR, PT1X, PT1Y,
PT1Z, PT2X, PT2Y, PT2Z, iR,iG, iB |
|
NAME: name
of Cutting Line to be registered
DIR: orientation
of graphic output
= NORMAL: produce the
graph normal to the plate elements
= INPLANE:
produce the graph in the in-plane direction of the plate elements
PT1X:
starting point of the Cutting Line
PT2X: end
point of the Cutting Line
iR: color
number of Red
iG:
color number of Green
iB: color
number of Blue |
|
*CUTLINE2 (Plate
Cutting Line Diagram) |
|
Graphic output of internal forces of plate
elements along a cutting line |
|
; NAME, DIR, PT1X, PT1Y,
PT1Z, PT2X, PT2Y, PT2Z, PT3X, PT3Y, PT3Z, iR, iG, iB |
|
NAME: name
of Cutting Line to be registered
DIR: orientation
of graphic output
= NORMAL: produce the
graph normal to the plate elements
= INPLANE: produce the
graph in the in-plane direction of the plate elements
PT1X:
starting point of the Cutting Line
PT2X: Coordinates
defining the local x-direction vector
PT3X: Coordinates
defining the local x-y plane vector
iR: color
number of Red
iG: color
number of Green
iB: color
number of Blue |
|
*UNKCONS (Unknown
Load Factor Constraints) |
|
Specifying the constraint conditions to
be satisfied by the load
combination results, which include unknown
load factors |
|
; NAME, TYPE, iID, iPOINT,
iCOMP, COND, bVALUE, VALUE, iOBJ |
|
NAME: name
of the constraint conditions
TYPE: type
of the constraint conditions
=
REAC: Reaction
= DISP: Displacement
= TRUSS: Truss force
= BEAM: Beam force
iID: node
(cooresponding element) number
iPOINT: selection
of the location of the member force
iCOMP: selection
of the member force component
COND: Equality/Inequality Condition
= LE: Less than or Equal
to
= EQ:
Equal to =
GE: Greater than or Equal to
bVALUE: option
to enter Value (YES/NO)
VALUE: value
to be satisfied for the reaction component
(displacement component,
member force of truss or beam)
entered
in the load combination, which includes unknown load factors
iOBJ: Other
Node |
|
*UNKFACTOR (Unknown
Load Factor Data ) |
|
Creating new unknown load factor groups
by entering the conditions to
obtain unknown load factors |
|
; NAME=NAME, LCOMB, FTYPE,
SIGN ;
1st line
; UNKCONS1,
UNKCONS2, ..., UNKCONSn
;
2nd line
; LCNAME1,
WF1, LCNAME2, WF2, ... ;
from 3rd line |
|
NAME: name
of the unknown load factor group
LCOMB: load
combination used to calculate the unknown load factors
¡Ø the load combination
for calculating the unknown load factors must include
the load conditions determining
the load factors
FTYPE: selecting
the composition method of object fuctions composed of unknown
load factors
= LINEAR: load factor?the
linear sum of the absolute values of the weight factors
= SQUARE: load factor?the
linear sum of the squares of the weight factors
= MAXIMUM:
load factor?the max value of the absolute values of the weight factors
SIGN: assignment
of the signs to the values calculated for the unknown load factors
= NEG: assigns the range
of the value to minus (-)
= BOTH: assigns the range
of the value to all ranges
= POS: assigns the range
of the value to plus (+)
UNKCONS1: constraint
conditions to be satisfied by the load combination results,
which
include unknown load factorsLCNAME1: name of load case used as the
unknown load factor
WF1: scale
factor, which is intended to adjust the relative importance of the
object function by assigning
a weight factor to an unknown load factor |
|
*BATCHCVT-MVLTRC (Batch
Conversion from MVLRC to Static Load) |
|
A number of loading conditions of different
moving load locations are converted
into static loadings and produced as model
files of the MCT type. This is an extremely ]useful
feature when a number of loading conditions
need to be converted. Conversion
is carried out by loading locations, result
types, etc. all at once. |
|
; NAME=NAME, TYPE ;
1st line;
:NODE_OR_ELEMENT_LIST
;
2nd line
; bPART_I,
bPART_1_4, bPART_1_2, bPART_3_4,
bPART_J ;
3rd line
; bFxx,
bFyy, bFzz, bMxx, bMyy, bMzz, bVxx, bVyy
;
4th line
; MOVING_LC1,
MINMAX1, ... , MOVING_LCn,
; MOVING_LC1,
MINMAX1, ... , MOVING_LCn,
MINMAXn ;
from 5th line |
|
NAME:
the name of the batch conversion
TYPE: Type
of result
REAC:
Reaction
DEFORM:
Displacement
TRUSS_F:
Truss Forces
Beam_F:
Beam Forces
Plate_F:
Plate Force
Beam_S:
Beam Stresses
NODE_OR_ELEMENT_LIST: The
list of the elements and nodes to be converted
bPART_I: the
i-end of the beam element
bPART_1_4: the
1/4 position of the beam element
bPART_1_2: the
1/2 position of the beam element
bPART_3_4:
the 3/4 position of the beam element
bPART_J: the
j-end of the beam element
bFxx:
Fxx of the plate element forces
bFyy: Fyy
of the plate element forces
bFzz: Fzz
of the plate element forces
bMxx: Mxx
of the plate element forces
bMyy: Myy
of the plate element forces
bMzz: Mzz
of the plate element forces
bVxx: Vxx
of the plate element forces
bVyy: Vyy
of the plate element forces
MOVING_LC1: the
dynamic load condition results to be printed
MINMAX1:
Min/Max of the dynamic load conditions |
|
*HYD-NODE (Heat
of Hydration Node ) |
|
Specifying the directional component of
the nodes and stresses for which
the time history analysis results of a
heat of hydration analysis will be produced |
|
; NAME, iNODE, iCOMP |
|
NAME:
name of the graph of the time history analysis
iNODE: node
number
iCOMP: stress
component
= 0 : Sig-XX
= 1 : Sig-YY
= 2 : Sig-ZZ
= 3 : Max (X, Y, Z) |
|
*COLUMN-SHORTENING
(Column Shortening ) |
|
Produce graphs for column shortening of
a highrise structure resulting from a construction
stage analysis |
|
; NAME, X, Y, TOL, DISP-TYPE,
CONST-STAGE |
|
NAME:
the name of the graph
X,
Y: the location of the column in the global coordinates X &
Y
TOL:
the allowable tolerance
DISP-TYPE:
type of displacement
CONST-STAGE:
displacement resulting from a construction stage |
|
*LOCALDIR-FSUM (Data
for Local Direction Force Sum) |
|
The load conditions and combination results
of the local coordinate |
|
; NAME=NAME, MODE, ANAL,
LCB, TOL, bZVECTOR,
ZVX, ZVY, ZVZ ;
1st line
; X1,
Y1, Z1, X2, Y2, Z2, X3, Y3, Z3, ... ;
from line 2 |
|
NAME: load
case
MODE: the
method of selecting the subject plane that includes the nodes
where internal forces
are to be combined}
ANAL:
types of loads
LCB:
load case
TOL:
tolerence
BZVECTOR: Enter
a vector to define the z-axis of the local coordinate system to
which Result Output is
referenced (YES/NO)
{NO}
ZVX:
the x-coordinates of the vertical vector of the surface
ZVY: the
y-coordinates of the vertical vector of the surface
ZVZ: the
z-coordinates of the vertical vector of the surface
X1: the
coordinates of the first node in the x- direction in the global coordinate
system
]Y1: the
coordinates of the first node in the y- direction in the global coordinate
system
Z1:
the coordinates of the first node in the z- direction in the global coordinate
system
Y2: the
coordinates of the second node in the y- direction in the global coordinate
system
Z2: the
coordinates of the second node in the z- direction in the global coordinate
system
X3: the
coordinates of the third node in the x- direction in the global coordinate
system
Y3: the
coordinates of the third node in the y- direction in the global coordinate
system
Z3:
the coordinates of the thi |
|