Learning Forum

[alma anila]

Hi, 

I have a model which I expanded with thermal expansion. Now I want to use this expanded model (taking the stress-strain results) and apply compression by adding a fix base. How can I use the stress-strain results of this first model as the initial time step of the second analysis using Ansys WB. I tried adding step 2 but this doesn't let me add the boundary conditions only for the second step. When I do 2 step analysis and add the fixed base, it adds it to both steps. I just want to take the stress-strain results of the first model. How can I do this? 

[mohan.urs]

Hey Alma Anila,

Instead of using fixed support in the second step compress it using a displacement boundary condition, and deactivate the displacement boundary condition in 1st step.

In the above you can see that I've deactivated the displacement in 1st step. Just Right click on that particular step and you will see the option to deactivate it. The blue highlight also proves the same in load diagram.

[alma anila]

Thank you for your reply. However, it did not work for me. Base nodes changed location (in step 1 with thermal analysis) so I can not make them zero displacement in step 2 even if I deactivate the first step. Would it be possible to share the model with you?

[mjmiddle]

You could apply the displacement in a command snippet in the second load step which gets each node's current location, then uses the D command to set the same displacement.

As far as using strictly workbench and Mechanical GUI-allowed abilities, link Solution cell to Model cell. You will also link an "External Data" to the downstream "Setup cell":

In the upstream model, you right click on the 3 X, Y, Z normal stresses and 3 XY, YZ, XZ shear stress to "Export Text File":

In the External Data system, one file must be marked as Master:

Insert an initial stress under the imported load folder in Mechanical. Alternatively, you could have exported strains and inserted an initial strain in Mechanical. You should not use both since this can cause overconstraint.

When Solution cell is linked to Model cell to transform deformed geometry, the initial stress import “Weighting” only accepts "direct assignment" import no matter whether “Mapping Control” is set to “Program Controlled” or “Manual.” This matches up data at node IDs, so you must only tag the node Id column and stress value column.

(When deformed data is transferred through an unlinked method, such as through STL, pmdb, cdb, you will be able to set mapping methods, instead of direct assignment, and you must specify the X,Y,Z locations column in the "External Data." You will need to use a command snippet to export the 6 stress components at the deformed locations.)

In the “Imported Initial Stress” in Mechanical you must set the 6 columns:

[alma anila]

Thank you so much, this is very helpful. I have a couple of follow up questions to solve my problem:

-       1. I did a thermal analysis and I want to import the thermal strains (not plastic or elastic) as my initial condition. The option you explained only let me import plastic or elastic strains as initial strains. Is there any way to map thermal or total strains? I need EPTT or EPTH’s 6 components instead of EPEL’s or EPPL’s. Because my EPEL and EPPLs are zero. However, WB only gives the options plastic or elastic strains when inporting.

-       2. You said “Alternatively, you could have exported strains and inserted an initial strain in Mechanical. You should not use both since this can cause overconstraint.” However, I need both mechanical stresses (caused by expansion) as well as thermal strains as my initial conditions. Is it possible to import both?

-        3. After following what you did and importing stresses, I defined my new boundary conditions and load and ran my analysis. However, the stress-strain results I get do not start from the values imported. I would assume that at the initial time step I would see the imported value then it would change according to the load applied. However, adding boundary condition to the model immediately changes the stress-strains of all nodes. Any idea what might be the reason?