Mecway v4 solver vs. Calculix v2.8 solver

VMH

Just a comparison using linear static analysis with linear elastic material (attached).

Would someone show me a few screenshots of how to add material nonlinear using the new features for CCX for this model as an example(also attached).

Material (stress-strain curves):
Yield Strength = 36ksi at 0.2% strain
Ultimate Strength = 58ksi at 20% strain

Victor

Here you go. I deleted the existing material and added a custom model definition section with a plastic material for bilinear hardening like this. I also doubled the load to make it exceed the yield stress in some places.

*SOLID SECTION,ELSET=Meshed_Geometry,MATERIAL=MyMaterial
*MATERIAL,NAME=MyMaterial
*ELASTIC
125e9,0
*PLASTIC
250e6,0
400e6,0.198

Where the numbers came from:
125e9 Pa is the elastic modulus = 36ksi/0.2%
0 is the Poisson ratio. You might need to change this.
250e6 Pa = 36 ksi is the stress at 0% plastic strain (0.2% strain).
400e6 Pa = 58 ksi is the stress at 20% total strain.
0.198 = 20% - 0.2% is the plastic strain where stress is 400e6 Pa.

Now, there is something in the meaning of these numbers that I'm not entirely sure of. The plastic strains should really be "effective plastic strain" so you may need to check the CCX manual to see if that's significant.

VMH

Victor,
Thanks for your help!

Victor

I notice you changed the "equivalent plastic strain" (not effective as I wrote earlier) from 0 and 0.198 to 0.002 and 0.2 respectively. Is this because of the "equivalent" part? From what I understand, you should subtract elastic strain from total strain to obtain plastic strain. It probably doesn't make any significant difference for this material though.

VMH

It was to be consistent with the test I couldn't get the units to come out correctly that I also posted in the Version 4 Beta thread. I will be looking into CCX manual and correct them. Thanks for point them out and help on this.

VMH

Victor,

See attachments.

I did a test on quadratic shell elements model solving with Mecway and CaliculiX solvers. The results are about the same. However, I noticed that the number of nodes in the results of CalculiX solvers increased and also the result plots appears to have "solid" elements (with thickness shown). Also attached is .liml file for reference.

Let me know of your thoughts. Thanks

Sergio

Hey, nice model VMH! As far a I know CCX expand the shells to solids, have you try to postprocess the results file (.frd) in CGX to see if you see as a shell or solid?

For small models like that I preffer to use a solid mesh (extruding the shell in the element normal direction in Mecway) in order to avoid this kinf of issues when postprocessing.

Regards

VMH

The purpose for this model was trying parametric modeling in FreeCAD for surface modeling. For this model, I can change any dimensions and any referencing dimensions to that dimension will also update. For example, if I can the diameters for the braces, all of the cope on the chord will also update, etc.

I didn't try CGX yet (I'm not familiar with it).

Victor

CCX outputs shell elements as solids by default. You can turn this off in Mecway by adding a custom step contents containing

*EL FILE,OUTPUT=2D

VMH

Victor, Thanks

Stefanos

I have used the *EL FILE,OUTPUT=2D, solved with CCX and get strange results compared to previous results from CCX without the *EL FILE,OUTPUT=2D, did I misunderstand something?

Victor

I see the same alternating stress by opening the .frd file in CGX. I think this is a CCX issue that you could ask about on the CCX forum

https://groups.yahoo.com/neo/groups/calculix

Bear in mind that OUTPUT=2D removes out-of-plane bending stresses on shells by averaging the stress on both sides so it's only really useful if you've got a genuinely 2D problem like this one.

Stefanos

Hi Victor,

I see.., but anyway in the case above, implementing the *OUTPUT=2D the stress results on each side have NOT been averaged, but rather were added! (40 vs 104)!

Victor

You're right, it is adding them! I'd bring this up on the CCX forum. I seem to remember it has a bug with OUTPUT=2D on beams too so I'd guess that's a little used and poorly tested feature.

Stefanos

OK, thanks Victor

Stefanos

In this rough test example, whilst deformation and stress between MECWAY & CALCULIX is about the same, the buckling modes have 100% difference (calculix has the half value than mecway). I have in mind the difference due to elements type and different solver, but 100% is still a very large difference. Any comments are welcome - thanks

VMH

Stefanos,

Mesh convergence is importance. First try a courser mesh and then try with a finer mesh. If the results difference between the two are not significant then your coarser mesh would be adequate.

For your model, I refined (2x) the plate and rerun with Mecway and CCX solvers. The results were about the same for linear static analysis. As for buckling, they are close but not the same. Maybe refine the mesh one more time may get the results closer or about the same. See attachments.

Also changing the "Shift Point" closer to the buckling factor may be more accurate or may be about the same. I didn't try that.

Stefanos

Hi VMH, thank you for your reply.

Indeed, with the finer mesh the difference is much more reasonable.
Although the first mesh wasn't so coarse, especially the shell element proved to be quite stiff for this configuration, especially near the beam side, causing a much more higher critical value.

VMH

Take a look at this test of a coaser mesh using Quad8 elements instead.

Stefanos

Interesting, MECWAY results are close?

VMH

See attachments. They come out about the same but CCX solver were coming up with some lower number though.

Stefanos

Yes are close, but as far I can see, in every pair of images the MECWAY solution has finer (double) mesh than the solution with CCX, is that right?

VMH

CCX convert the quadratic shell to quadratic solid. So in all cases, we are not comparing "apples" with "apples". I don't use eigenvalue (linear) buckling for real world problems since they are usually not conservative except for using the displacements for the mode shape as initial imperfections for the nonlinear buckling analysis. Best wishes on comparing eigenvalue (linear) buckling between the two solvers.

Stefanos

Both cases results in min acr, so we comparing apples with apples (acr vs acr). I don't comparing the different solvers or elements. Is about using the right element (good result with minimum nodes). Regarding linear buckling analysis (min acr) is a fundamental analysis in EC3 for steel structures (for real world problems, but with further processing/calculation), you may see if you want, the procedure of the general method of EC3 - global stability analysis of structural elements by the general method as specified in EN 1993-1-1 (6.3.4). - Thank you for your time.

VMH

There are many references on this topic (Here is one: https://wiki.csiamerica.com/display/kb/Eigenvalue+vs.+Nonlinear+buckling+analysis). Don't mind my comments. Each person is welcomed to do whatever the design required. Thanks

Stefanos

I know the ''Eigenvalue vs. Nonlinear buckling analysis'' topic. As i said before, EN 1993-1-1 (6.3.4) sets out the procedure that should be followed. Thanks anyway

EDIT: For avoiding misunderstandings a full 3d GMNIA is the ultimate analysis - no one argues against that - but yet not feasible/practical for every day work/design (construction industry speaking), so seeking for valid alternatives, involving linear bifurcation analysis and EC3 expressions, as i mentioned above.