Questions and Answers

A1. Here is the explanation about plasticity in concrete with midas Gen.

 

One parameter models

Under tensile stresses, concrete will fail by a brittle fracture with very little plastic before failure.

Associated fracture criterion: Rankine (Maximum tensile stress criterion)

This is not supported in midas Gen.

 

Under high hydrostatic pressure (compression), concrete can yield and flow like a ductile metal on the failure (or yield) surface.

 

Hydrostatic pressure

 

For metals and for concrete in the high pressure range, the effect of hydrostatic pressure on the yield value of material may be neglected. It follows that shearing stress must be the major cause of yielding.

Associated yield criterion:

-          Tresca yield criterion (Shear stress criterion)

-          Von Mises yield criterion (Shear stress criterion)

This can be simulated with midas Gen.

 

Two parameter models

In the intermediate stress range, the failure criteria of concrete are sensitive to hydrostatic pressure.

Associated yield criterion:

-          Mohr-Coulomb criterion

-          Drucker-Prager criterion

 

Mohr-Coulomb criterion

 

The failure is governed by the equation below.

c (cohesion) and φ (internal-friction angle) are determined by experiment. This equation is referred to as the Mohr-Coulomb criterion.

c (cohesion) becomes equal to the yield stress in pure shear. c = fc’/sqrt(3) = 4000 psi/sqrt(3) = 2309.4 psi

From the test, m = (1+sin φ)/(1-sin φ) = 4.1. Thus, φ=37.4 degree

The stiffness after yield point can be defined by Hardening Coefficient. The zero value of coefficient represents perfectly plastic or zero stiffness.

The option of hardening rule: Isotropic, Kinematic, Mixes. Hardening rules describe how this yield surface changes in shape as yielding occurs.

 

Isotropic: Expansion of the yield surface. This is meant for proportional loading only.

 

 

 

Kinematic: Translation of the yield surface. This is meant for cyclic loading.

 

Mixed: Translation and expansion of the yield surface

 

Note that material nonlinear analysis in midas Gen does not take into account the unloading and reloading. It is recommended that proportional monolithic loading is tried with the Isotropic option.

A1.

Algorithm of Beam’s semi-rigid release boundary by relative ratio or specified values

In case of 2-Dimensional stiffness of Beam element, if we disregarding shear deformation, Beam element stiffness matrix can be shown below equation.

 

In order to incorporate semi-rigid boundary condition, we add additional node A and 2node spring stiffness matrix which is constituted by rigid stiffness and specified stiffness. Rigid stiffness value is defined penalty method and specified stiffness is defined by user’s input: ratios or values.

The total dofs size of K matrix can be expanded to 18 or 24 dofs. If we condense beam end dofs(uB,ΘB), the dofs size will be reduced to 12 dofs. In this condensation, including load vectors is needed.

In case of a relative type semi-rigid connection, the Ksp is defined by multiplying the factor to the related element stiffness value.

The other unchecked(in the dialog) components’ stiffness are defined by penalty method.

BIG/(BIG+1) = 0.999990000999… : There is no reference. This is from a kind of engineering experiences.

A1. For the specified displacement, midas uses the penalty method. According to this method, the solver internally creates a very stiff spring at the node to which displacement is specified. The stiffness of the spring is determined as about 10⁴ times the largest value of stiffness matrix of structure. And then the solver applies a load to the spring, the amount of which is equal to the product of spring stiffness and the specified displacement. Therefore, the same displacement as the specified displacement will occur at the node.

This method has an advantage that the calculation is effective when there are many load cases. But it may be that the sum of reaction is not exactly zero for the specified displacement load case, which is generally negligible. If the stiffness of spring is further increased more than 10⁴ times, the summation of reaction will be closer to zero. On the other hand, the increase of the stiffness of spring might cause some other problem in the FEM analysis e.g. numerical error.

There is no setting in which this can be controlled by the user.

A1. Deflection Amplification Factor (C_d) amplifies the drift computed using elastic analysis in order to account for the drift due to inelastic response of the lateral force resisting system (LFRS). As general philosophy of earthquake resistant design, the structure is designed for the lower amount than the actual force which it will be subjected to during actual earthquake. Because we rely on nonlinearity hence we reduce the actual force by dividing Response modification factor to get the design force in Response Spectrum Analysis or Static Seismic Analysis. But the displacement of the structure will be according to the actual force. Hence, the displacements obtained are multiplied because of reduced forces by that response modification factor. This factor is specified as per ASCE/SEI 7-2010 (American Society of Civil Engineers/Structural Engineers Institute). Therefore, the factor was included in the serviceability parameters. If user is using design code other than ACI and he wants to amplify the deflection as per the above reason, then the deflection amplification factor may be used. Otherwise, it may be used as 1 by default.

A1. For using Import feature for the load combinations in midas Gen you need to manually create *.lcb file which will later be imported. The format of the *.lcb file is as follows.

Sequential number, combination method, unit load case i, load factor i, unit load case j, load factor j, ..., load combination k, load factor k, load combination l, load factor l

Examples)

1, , 1, 1.0, 2, 1.0

2, , 1, 1.4, 2, 1.7

Note Combination methods

blank,0	: Add
1	: Envelope
2	: ABS
3	: SRSS

Rather than importing using the import option we also have two other alternatives for importing the load combinations from one file to another. You might be knowing them already but I believe its worth mentioning.

1) Copy and paste feature is supported for the load combinations in the Spread Sheet Form. In this form by correctly copying the cells from one model file you can paste it into other model file.

2) You can export the model as MGT file and from there you can copy the load combinations. By pasting the load combinations in another model file's MGT command Shell and clicking run, you can get the load combinations imported.

A1. In order to obtain the results of Plate Force (Unit Length), we need to  understand the following diagram.

The program has the stresses at the nodes of the plate elements. These stresses are then integrated in the following manner to obtain the desired results.

A1. Deflection Amplification Factor (C_d) amplifies the drift computed using elastic analysis in order to account for the drift due to inelastic response of the lateral force resisting system (LFRS). As general philosophy of earthquake resistant design, the structure is designed for the lower amount than the actual force which it will be subjected to during actual earthquake. Because we rely on nonlinearity hence we reduce the actual force by dividing Response modification factor to get the design force in Response Spectrum Analysis or Static Seismic Analysis. But the displacement of the structure will be according to the actual force. Hence, the displacements obtained are multiplied because of reduced forces by that response modification factor. This factor is specified as per ASCE/SEI 7-2010 (American Society of Civil Engineers/Structural Engineers Institute). Therefore, the factor was included in the serviceability parameters. If user is using design code other than ACI and he wants to amplify the deflection as per the above reason, then the deflection amplification factor may be used. Otherwise, it may be used as 1 by default.

A1. The governing Load Combination for Shear Design is not decided on the basis of the magnitude of the shear force. The governing load combination is decided on the basis of the ratio of the shear force and shear capacity.

Now, if there are two shear forces V_Ed1 and V_Ed2 such that V_Ed1>V_Ed2. V_RDs (Shear Strength provided by steel) and V_Rd,c (Shear Strength provided by concrete) will be calculated. If V_ED1/V_Rd,s is less than the V_ED2/V_Rd,c, the V_Ed2 will be used for shear design, even if V_Ed2 is smaller of the two shear forces.

A1. When I run the steel optimal design for your model, I get the following table.

As you can see that the section 1 has Combined Stress Ratio of 1.242 >1 (Allowable ratio). Thus you would go for optimization of this section. D1 value shown buy the software for this section is 0.656. When you click on Design & Analysis the software would look for sections with the depth of 0.656(+/- 5%)m only and it will present the optimal sections by iterative analysis and iterative design. Since there is no other section with this depth which can have a combined stress ratio within limits, the software can find the most optimum section of W8x40 in your model as shown below.

But this section doesn’t has the Combined Stress Ratio <1. Thus I would recommend you to change the D1 value to zero. Doing so the software will look all the sections as per the database of the code.

You observe a message stating “Section is not changed” when the ‘Number of Repetitions’ under Analysis Option are specified more than required. Getting this message is not a concern since it just indicates that the software has already found the most optimum section in previous iteration and thus the section is not changed. See the image below to view the number of repetitions I am talking about.

A1. I looked into your model and I can say that the modelling seems to be fine. The reason for obtainment of the warning message stating the inability to find the performance point is the definition of the 5% damped response spectrum.

You are trying to perform pushover analysis using Procedure-A. Below is the explanation for the procedure adopted by the software for this procedure.

1) Transform the capacity curve into a capacity spectrum. This is done in software by clicking "For Performance Point (FEMA)". Clicking this, the Base shear vs displacement curve is converted into Sa by Sd curve.

2) Develop the 5% damped (elastic) response spectrum appropriate for the site. This is done in the software by clicking onto "Define Elastic Spectrum". Before you click this option the software automatically finds out one response spectrum function for which it shows the performance point.

3) Software selects a trial performance point api, dpi (on the capacity spectrum) and for that a bilinear representation is developed internally. In your model file, you are not getting any performance point for the automatically defined spectrum and not for some other spectrums from the database as well because, the software is unable to find a trial performance point for which the demand spectrum would intersect the capacity spectrum (shown in the image below).

4) Software calculates the reduction factors using which it obtains the demand spectrum. If this demand spectrum intersects the capacity spectrum within acceptable tolerance of 5% then that point is considered to be the performance point. Demand spectrum can be obtained for various inherent damping of the structure (shown in the image below for response spectrum defined as per IS standards and inherent damping of 2%).

 

The point where the green line (demand spectrum) intersects the yellow line (capacity spectrum) is the performance point.

 

A1. Masonry material is not supported for Wall element in midas Gen since the wall is RC/CRB (Reinforced Concrete OR Concrete Retaining Block) wall.

MIDAS Gen supports idealization of the masonry structure as an equivalent frame easily allowing to introduce other structural elements, such as reinforced concrete beams or columns, together with the masonry ones. Thus, it appears particularly versatile to model also mixed structures (e.g. mixed masonry and reinforced concrete structures which are quite common in existing buildings).

In the EFM (Equivalent Frame Model) the masonry wall is modelled with Piers and Spandrels connected through rigid link. For more information on modelling the equivalent frame model you can go through the research papers on EFM available online.

A1. The reason for hanging of GSD is the large section size (diameter = 8ft) and very small mesh size (mesh size = default mesh size = 0.1in). In order to perform the design using GSD, please increase the mesh size. Mesh size greatly affects the time required for design. Larger is the mesh size lesser will be the time needed for the design.

In order to change the mesh size go to Model tab and click on Section property. Software will take time but finally you will get the option for inputting the mesh size. By increasing the mesh size to 1in, I could obtain the design results successfully.