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
Comments
*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.
Thanks for your help!
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
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
I didn't try CGX yet (I'm not familiar with it).
*EL FILE,OUTPUT=2D
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.
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)!
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.
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.
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.