Learning Forum

[Ben_Ben]

I noticed I was getting no stress results for my simulation with Beams. 

Here is my sim. I am displacing the top node and constraining the bottom. Here are start and end states: 

But I get no stresses in my results. 

So I checked the "beam section results" box:

I checked the D3 files and changed beam to 1 for *DATABASE_EXTENT_BINARY, *DATABASE_BINARY_D3PLOT and *DATABASE_BINARY_INTFOR:

I also saw this link: https://lsdyna.ansys.com/beam/
So I used elform = 1 for beam formulation

I get this error if I run in Ansys LS-Dyna (via Mechnical in Workbench) and on HPC: 

[Jim Day]

Try setting BEAMIP to the total number of integration points for your beam cross-section. That number should be evident from looking at the variable QR in *SECTION_BEAM. For example, QR=2 (default) provides 4 integration points so BEAMIP should be set to 4 in that case.

[Ben_Ben]

My qr is -1 Will change it to 2

 

[Ben_Ben]

That gives me this error for all my elements:

 

[Jim Day]

If you change QR to 2, also change CST to 0. You'll then be modeling a square cross-section with dimensions 1.0x1.0 and 2x2 integration. Set BEAMIP=4. Do you get then get beam stresses in the 4 integration points?

[Ben_Ben]

My beam is a circular cross section. I can try the above though.

[Jim Day]

For circular, leave QR=2, set CST=1, and set TS1=TS2 to the outside diameter and TT1=TT2=0.

[Jim Day]

If you successfully get beam stresses in the modified model, we can go back and try to address the case of using a user-integration rule (*INTEGRATION_BEAM).

[Ben_Ben]

Hey Jim, 

I've done this and still don't get any stress results in beams.

Ben

[Jim Day]

I think this would be easy to debug if I had your input file, but unfortunately, we're not allowed to share files via the Learning Forum. See the notes in https://www.dynasupport.com/howtos/element/beam go into more depth than I have. See especially the last two paragraphs in those notes.

[Ben_Ben]

 

Maybe I’m missing something. I’ve had another run through and I can’t seem to find the issue. Quite confused because is a really simple model, one beam being displaced at one end and held at the other. I’ve attached a couple screenshots of the input file. Included all the relevant parts apart from the nodal and element data. Can you spot anything? 

 

[Jim Day]

The issue could be the way in which you're postprocessing the d3plot data. As a check, add *DATABASE_ELOUT and *DATABASE_HISTORY_BEAM so as to output beam data to the output file elout. Then try plotting axial stresses at beam integration points by reading elout into LS-PrePost using Post>ASCII>elout>Load. I'm assuming you're running SMP for this small model. Also, while debugging, I'd get rid of *DAMPING_GLOBAL and also set BEAM to the default value of 0 in *DATABASE_EXTENT_BINARY.

[Ben_Ben]

I added *DATABASE_ELOUT and *DATABASE_HISTORY_BEAM .

I also removing damping. 

But there is only beamip in *DATABASE_EXTENT_BINARY so I changed beamip to 0 

[Jim Day]

Leave BEAMIP set to 4. Rerun. Postprocess elout with LS-PrePost to get axial stress or just open elout with a text editor to check for stresses. I'm assuming you're running SMP LS-DYNA and elout is written as an ASCII file.

[Ben_Ben]

This worked:



I now have a plot for each element, for each integration point. Thank you for your help.

So going forward I need to read stresses for beams through the elout method? 

[Jim Day]

Great. That was just a check to make sure beam stresses were being output. You should be able to get the stresses from d3plot as well. When you postprocess d3plot with LS-PrePost, make sure you've selected "Beam" if creating fringe plots or "Etype: Beams" if plotting time histories.

[Ben_Ben]

Amazing, is working with fringe plots and plotting time histories. 

Is still not working in Workbench LS-Dyna. But know I know how to access via LS-PrePost its ok. 

Thanks for your help!