I am having some problems to understand the results about the strains. I did not find in the help the difference between :
- solid von mises strain
-solid non linear von mises strain
In fact I run an analysis (sol106) with a part of linear elastic material properties. I check the strains there and they are different. I assumed that non linear strain should be 0. I show the results from FEMAP for one output location
Value = 0.0004411 | Output Vector 70861 : SolidC5 Von Mises Strain
Value = 0.000436 | Output Vector 70983 : Nonlinear SolidC5 Von Mises Strain
Value = 0. | Output Vector 70984 : Nonlinear SolidC5 Plastic Strain
As It should be plastic =0
NASTRAN reports linear strain in the global coordinate system, nonlinear in elemental. Use the Transform option in the PostProcessing Toolbox to transform everything to global and then you can visualize them in a consistent frame of reference.
I did it but it does not work. My model in this area (aother areas have plastic defintion) is elastic, so the only nonlinearity could be due to large displacement .
The issue is: what does it mean?
1.solid von mises
2.solid non linear
I tought that:
1.solid von mises : total strain (elastic+plastic)
2.solid non linear:???
3.solid plastic: it is clear, the plastic part
So in my example as 3 component is 0. Solid non linear due to large displacement should be 0 . total strain=elastic part
It seems to be that sol 106 only obtains the stresses at the centroid and the corner values are extarpolations from FEMAP. This is the reason, I think, of some discrepancy. At centroid the values match always
If some developer from siemens can confirm that . Because I can not find this issue in the help
The primary source of this confusion is that Nastran outputs 2 stress datablocks from nonlinear SOL 106. This really highlights a critical point for solid element models, the 2 stress datablocks from Nastran are reported and stored in 2 different output coordinate systems.
The user must be aware of which vectors he is displaying and the orientation of the stress results.
In Femap, stress/strain result vectors with the "nonlinear" label are in the element coordinate system.
The other stress/strain result vectors are in the material coordinate system.
This point is critical when the user decides to use transformation to view the results in a meaningful and consistent plot. The Femap default for the transformation basis is the linear assumption "material" system. If the user is transforming the "nonlinear" results vectors then he must reset the basis to "element" system as shown below:
Continue reading for more details on the 2 datablocks
The first datablock from Nastran is the nonlinear stress/strain datablock.
This nonlinear output is controlled by the case control command NLSTRESS and is created if large displacement or nonlinear materials exist in the model. If you have asked for printed output, then in the f06 file you will see results with the following format and header:
Notice there is both stress and total strain data as well as "equivalent stress"(von mises) and plastic strain, but Nastran does not calculate the principal stresses in this datablock.
In Femap all of the result vectors from this datablock have "nonlinear" in the label. Notice that by default Femap actually calculates the additional principal stress/strain results highlighted in blue from these nonlinear vectors. All of these results labeled "nonlinear" in Femap are reported in the element coordinate system from Nastran and stored as such in Femap.
Nastran also outputs a second datablock of "linear stresses". This output is controlled by the STRESS case control command. Nastran uses the converged nonlinear displacements but the linear stress data recovery module is used so the output is formatted the same as a SOL101. If you requested printed output you will see the following format and header:
These "linear stress" results are reported from Nastran and stored in Femap in the material coordinate system.