I am a beginner in Femap. I have defined the following 'vs Stress' curve for a steel plastic material model:
0.002 (0.2% ) 300 MPa
0.2 (20% ) 500 MPa
1 (100% ) 500 MPa
I had expected that the von Mises stress results would in any case be less than (or equal to) 500 MPa for the above definition which is not the case in my model. Am I missing something in the material definition?
two simple answers:
- what solver did you use? sol 101,sol 106...
- did you get plastic strains?
because I think if the property is set with the material you defined (it seems to be ok), the problem is that you are solving with the linear solver and then nonlinear issues are not taken into account
Ok. A this point and assuming that you get plastic strains, that means that the solver and property section with the appropiate material is being read by the solver. So with no more info I can not understand why you are getting higher stresses than VM. The solver should be follow the curve.
Mabye some pictures could help to understand the problem. I supposed that the problem has converged and in the model all the properties are defined with the same material. No elastic material properties
The model has two solid components connected with a bolt (modelled as a beam element and connected to each solid using rigid spider elements). The solids are non-linear steel but the bolt material is linear steel (E = 210GPa and nu=0.3).
I have created a group for solids and only this group is activated when I make the stress plots. Could it be possible that it is somehow including the bolt stresses also?
It could be. Only activating the group is not enough. You have to choose contour options /contour group select the group of solid elements and put contour group. Maybe you have already done it.
I tried the steps you suggested for the contour options but it doesn't give the desired results. I think since I am an absolute beginner in Femap there is some setting in the material definition which I haven't set correctly.
I simplified the model (just one solid with supports on one surface and force on the opposite surface) and still the von Mises stress crosses 500MPa. I have attached snapshots from the material definition settings. Do you see something which could be the source of error?
I do not see any mistake. But I would trie first with elasto -plastic option defining just the yield with 500 and see the results. Some plots of Von Mises and plastic strain would be nice
The results may not follow the input stress-strain curve exactly because of the extrapolation from the integration points to the grids or element centroid. The integration point values can be printed in the ‘.f06’ file, but cannot be displayed in post processing.
For more direct comparisons it may be useful to look at gauss point stresses rather than the nodal values.
Take a look to this post where I explained how to select in FEMAP stress-strain output at GAUSS points with SOLID elements.