|
*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: poissons 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: poissons 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: poissons ratio for steel
POIC: poissons 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 isValue
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 : Ⅰ, Ⅱ, Ⅲ, Ⅳ, {Ⅰ}
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 (Ⅱ)}
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 elements 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: poissons 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: poissons 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 ≤ 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
※ 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
|
|