Ansys Workbench nonlinear plastic analysis 1

[omnnet]

Hello.

I'm stuck in this problem. I need to work in Ansys Worbench in the nonlinear plastic deformation. However I'm not having good results.

I'm trying to reproduce some analytical solved problem in the program, like the WBVMMECH029 problem of the Workbench verification manual. However I'm not getting the same results.

Can please somebody help me. I'm getting a lot of problems in the nonlinear simulations. The mesh real makes the difference but I need to understand the way to make the nonlinear simulation for
different shapes that aren't solved analytical anywhere else, so I need to get sure in the results.

I've already try a big lot of different configurations, but unsucessful yet. The very first problem is even out of Ansys, because is not easy to find a nonlinear exercise result that I can compare with the numerical results.

Thanks in advance for your time and help.

Best regards.

 

[flash3780]

The analytical solution for the elastic-plastic beam-bending problem in WBVMMECH029 is as follows (assuming perfectly plastic behavior):
M = sig_y*(3H^2-4c^2)*B/12

http://stuff.mit.edu/afs/athena/course/2/2.31/

http://www/fall01/beam.pdf

How far is your answer from the analytical solution? You wouldn't expect them to match exactly.

//signed//
Christopher K. Hubley
Mechanical Engineer
Sunpower Incorporated
Athens, Ohio

 

[omnnet]

Hello.

Thanks in advance for your reply!

I used the theory present in Tymoshenko book, present in the WBVMMECH029 reference.

The calculus really say that for a rectangular cross section beam, the Moment that make it enter in the plastic area is the 24000 lbf.in. Correct. However the book say, that the Moment that takes it to colapse, for these kind of beams is 1,5 time the initial moment. So as present there, 36000 lbf.in.

In the Ansys Workbench, after a lot of attempts I decided to change the "Element Control" to "Manual" and the "Brick Integration Scheme" into "Full". There I finally get to the +/- 36000 psi of the Equivalent Stress.

However the limit Moment before "not converged" takes me to about 31800 lbf.in in spite of 36000 lbf.in. This takes the Moment ration to 1.33 in spite of 1.5 like is present in Tymoshenko and some other books.

There are 2 curious things. Before I get to the "Element Control" changed to "Manual", for the 24000 lbf.in the stress was around 38000 psi!!!! Remember it says that the mesh should be about 0.5 inch for "element size". That's the 2nd curious thing. If I define the mesh to medium or fine, for the first moment 24000 lbf.in the stress take closer to 36000 psi, in other hand, the Moment of collapse gets smaller and not higher, so the ration won't be 1.5, not even 1.33, it's less than that.

Sorry If my explanation isn't clear, or make you more confused. About that link I found that pdf 2 days ago, but thanks for it too!

Best regards

 

[flash3780]

You're trying to collapse the beam? You'll have to turn stabilization on, and make sure that you have the large deflections option turned on as well.
Stabilization adds dashpots to the nodes in the model, so if it becomes unstable the model it help the model to converge.

//signed//
Christopher K. Hubley
Mechanical Engineer
Sunpower Incorporated
Athens, Ohio

 

[omnnet]

Thanks again! I'm trying to see if it collapses only near 36000 lbf.in (1.5 x 24000 lbf.in).

Large deflection is on, but I don't know how to turn on that Stabilization, how should I do it?

Best regards!

 

[flash3780]

If you're using Workbench v13, stabilization can be found under:
>> Analysis Settings >> Nonlinear Controls >> Stabilization
There are several stabilization options that you may try, but as usual, it's best to start with the defaults.
As I mentioned, stabilization adds dashpots to the nodes to help a quasi-stable analysis converge. It's good practice to compare the strain energy to the stabilization energy when post processing to ensure that the stabilization effects aren't giving you an erroneous result. If the stabilization energy is <10% of the strain energy you're probably in good shape.

If you have access to the Ansys customer portal, take a look at the Structural Nonlinearities training materials, which cover stabilization. The Ansys help files will also be able to elaborate on the different stabilization options and what they all mean.

Besides stabilization, you'll almost certainly want to turn on automatic time-stepping, which allows Ansys to bisect the load if it's having difficulty converging.

Good luck.

//signed//
Christopher K. Hubley
Mechanical Engineer
Sunpower Incorporated
Athens, Ohio

 

[omnnet]

Hello.

I've the 12.1. In Nonlinear controls only have:
- Force Convergence
- Moment Convergence
- Displacement Convergence
- Rotation Convergence
- Line Search

Best regards

 

[flash3780]

Best to double-check the help files, but I think that adding an APDL Command Snippet with the following does the same thing:

STABILIZE,CONSTANT,ENERGY,1E-4

You can add a command snippet with "Right Click" >> Insert >> Commands

//signed//
Christopher K. Hubley
Mechanical Engineer
Sunpower Incorporated
Athens, Ohio

 

[omnnet]

Done it, but still not converging.

Anyway, if I have to make all these changes for a nonlinear analysis in complex pieces in future, that I haven't make analytic calculus, I can never be sure of the results... That's by biggest fear...
The "Element Control" to "Manual" and "Brick Integration Scheme" to "Full" is something that I can accept for all nonlinear my future analysis, because I didn't find anything getting worst taking this options, it only gets more precise. But there still is the problem. I don't know what more to do to get a solution converging with a moment near to 36000 lbf.in.
I tried:
- Substeps
- Solver Type - Direct
- Shape Checking - Agressive Mechanical
- Element Midside Nodes - Kept
None of these made difference

I've found a very interesting way to analyse this beam (

https://confluence.cornell.edu/disp...2+-+Cantilever+Beam+-+Problem+Specification).

I just changed the material characteristics and turned ON the Large Deflection.

The good point is that the 1.5 times is really precise! 35900 lbf.in for example still converge. However that's anther kind of problem here.

The stress for 24000 lbf.in is 36000 psi! (Perfect)
For 30000 lbf.in is 45000 psi (WHAT?!) Bilinear Isotropic Hardening - Yield Strength= 36000 psi - Tangent Modulus= 0 psi. Why is it achieving 45000 psi?
For 35900 lbf.in is achieving about 54000 psi (same problem)
For 36000 lbf.in it collapses.

Thanks again for your time and help!

 

[omnnet]

Well, I got the solution (at least I think I did!).

If there is anyone with the same problem, for this exercise you just need to chose 2 things:

Element Control in Geometry - Manual
Brick Integration Scheme in Solid - Full

With the recommended mesh, you just need this to get more accurate results! However, still is a problem with the Moment ratio. For me it kept in 1,32. Well it's also solved, make a slightly blend in the face where the moment is applied and voila!

With a 0,025 inch of radius I got a moment ratio of 1.47!

Perfect!

Thanks a lot everyone, specially "flash3780" for your help!

About the line body I didn't got better results, but I don't need it now!