How to use existing solutions in subcases (Nonlinear static)?

[delaroca]

Hello!

Its been a while.

So, I'd like to know if there's a way to use an existing solution for a subcase in a Nonlinear static simulation with multiple subcases.

For instance, for a 2 subcases simulation consisting of:

• Subcase 1: Compression to 10 MPa (enforced displacement that gives that stress).
• Subcase 2: Loosening of 0.05 mm, or 0.03, or any other number I'd like to know.

I already know the results of the subcase 1, and that won't change for the next subcase. But currently, whenever I want to test a difference subcase2 scenario, I'm having to wait all the way for subcase 1 to complete.

Is there a way? I feel like there should be an easy way to set "that's the solution for this subcase, so just skip it".

Best regards,

Leonardo de la Roca

[John_Holtz]

Welcome back Leonardo!

The answer is yes and no.

• Yes, it can be done if you setup the analysis to do it.
• No in your case because you (most likely) did not setup analysis 1 to do it. 🙂  At the very least you need to rerun the analysis with subcase 1 one more time, and setup analysis 1 so that you can reuse the results from subcase 1 for every future analysis.

What you need to do is save the restart files when you analyze subcase 1. You can then have a separate analysis for subcase 2 read the restart files and "continue" the analysis. This article describes the steps: Creating a pre-stressed model for use in an additional analysis in Inventor Nastran.

I have not done a restart for a long time, but I think the results will be in two different files. The results from subcase 1 will not be in the model that analyzes subcase 2. If you need to look at both results, you can load each result separately to look at them. Or I'm sure you can use some magic to combine the two sets of results together using FNO Reader and workflow "Combine FNO". (The magic would be to rename the two results files to something0001.fno and something0002.fno.)

John

[jbarrong24EM3]

@delaroca

where you able to use the procedure in the Link that @John_Holtz John provided to solve the issue/question you had? if so, can you share a screen shot of how the NAS file was set up?

I tried to test something similar with a simple model, and unless I am misinterpreting the article the RESTART procedure on that link doesn't seem to do what it claims. 

Case-1 with (NLDATABASE=STORE) =48inch long 1inch diameter rod made of ASTMA36 Steel (Nonlinear material ON: Plastic option with failure occurring at .2 Strain) fixed at one end and -700lbs(Z_axis) load on the free end that results in stresses beyond yield and permanent deformation (max displacement ≈1.1"). 

Case-2=duplicate of case-1 with (NLDATABASE=fetch and NASTRAN NLINDATFILE ="appropriate path") = 48inch long 1inch diameter rod made of ASTMA36 Steel (Nonlinear material ON: Plastic option with failure occurring at .2 Strain) fixed at one end and -800 lbs (axial,X _axis) load on the free end.  Results do not show signs (max displacement≈ 4.11E-04 inches) of case-1 permanent deformation.

*edit  below  using

[John_Holtz]

Hi @jbarrong24EM3 

I have some questions and comments to clarify your analysis.

1. Based on the axial stress in the beam, the cross-section appears to be 1 inch radius, not 1 inch diameter. (That doesn't change any conclusions but might affect if you did any hand calculations. 🙂)
2. In case 1, you applied a 700 lb load that causes bending. Did you include a second subcase with 0 load so that you can measure the permanent deformation? In other words, if you only have 1 subcase, you know the deformation with 700 lb load is 1.1 inch but you do not know how much of that is elastic and how much is plastic. Once you remove the load, the bar may spring back to a permanent deformation that is surprisingly small. If you have 2 subcases where the load is removed, then the last result will be the permanent deformation.
3. In case 2, the axial load will try to straighten out the bar. If you output the results of all N increments in case 2, you should see the vertical displacement decrease from the permanent deformation to a smaller value. Are you seeing that?
4. This brings up another idea. In case 2, the analysis is static that responds only to the loads in case 2.
   1. If case 1 only has 1 subcase, the displacement of 1.1 inch is partly permanent deformation (let's say 0.1 inch for discussion) and elastic deformation (1.0 inch). In the first step of case 2 where there is no bending load and only a fraction of the axial load, the displacement is 0.1 inch from the permanent deformation plus the effect of the axial load.
   2. If case 1 has 2 subcases and the permanent deformation is 1.1 inch, then the first step of case 2 the displacement will be 1.1 inch from the permanent deformation plus the effect of the axial load trying to straighten out the bar. You should see the vertical displacement decrease as the axial load is increased.

Let us know what you find out.

John

[jbarrong24EM3]

@John_Holtz 
You are correct my rod has a radius of 1.

I reran model with higher loads subcase-1 -2000lbs and subcase-2 -1lbs to determine the approximate permanent deformation. And I was able to perform the restart using the axial load with no issues.

Thank you John.