Learning Forum

[Mo]

I'm doing a structural stress analysis in an assembly the steps I need to do are below:
1. The assembly will be under loads and temperature and get deformed.
2. New loads need to be applied on the deformed shape of step 1 without stresses produced in step 1. ( it is assumed that stresses made in step 1 relax over a long time)

I tried to export the deformed Geometry as .stl but repairing the .stl file is so time-consuming. Second way was I took the solution of step 1 and entered into a new analysis as below:

However, the beam elements twisted and rotated when I entered the Solution from one analysis (Step 1) into another (Step 2):

First step meshed Geometry:

Geometry entered in step 2:

the beam elements are connected to a few shell elements. the shell elements come to the 2nd step of the analysis very good but the beam elements twist and rotate.

Any solution or is there any way to do this any better?

thanks,

[mjmiddle]

Linking solution cell to Model cell would be the way to do it. I had submitted defect reports in the past on the beam cross section orientation changing between geometry, mesh, and postprocessing. Some were determined to just be display issues, and others the beam orientation was not able to be determined.

Exporting through STL would not be an option because it does not contain beam orientation. Since we can only set up beam cross section and orientation in DesignModeler, SpaceClaim, and APDL those would be the only formats you could go through if you wanted to export. Try a command snippet like this under Solution:

/post1
set,last
allsel
upcoord, 1
cdwr,db,defmodel,cdb

Then connect an "External Model" to a static structural and read the defmodel.cdb (in solution directory) to the "External Model" system.

[mjmiddle]

Here are a couple other ideas:

1. With solution linked to Model cell, set "File > Options >  Geometry > Beam Cross Section (for solver)" to "mesh" before solution in the upstream system.

2. Another idea would be to right click on geometry in the deformed system (solution linked to Model cell) and export the pmdb file. Open the pmdb file in DesignModeler, and you can reorient the cross sections on the beams for any that are wrong.