I have the following problem:
I am doing a nonlinear analysis (sol 106) with a material with the following values for the strain-stress curve:
I am expecting to get stresses less or equal than/with 400, whereas I get 630 MPa.
The problem is that when I am looking to stresses in the cartezian coordinate system, values are smaller that 400, but when I go to a cylindrical system, the values are big. Von Mises stresses are smaller than 400!
Solved! Go to Solution.
See If I undestand the problem:
- you run linear analysis and you get larger stresses (VM) than 400MPa. Then you perform non linear with yield 400 and then you get Von Mises larger than 400MPa?
You say that the reason of the 630MPA is because the components of stresses are large in cylindrical coordiante system. But VM does not depend on the coordinate system.
Hello and thank you,
I did only a nonlinear analysis (for th emoment). And yes, I got stress values greater that the last value on the strain-stress curve for tangential and axial stresses (it is a pipe). The VonMises stresses are smaller than the last value on the mentioned curve.
I do not know how the problem details but it seems to be that the components are larger than VM. But his happens only if they are in cylindrical???
If you run linear analysis then you can get the stress components and with them analytically you can obtain VM. VM does depend on the coordiante system. Either with cylindrical /basic rectangular should be the same. This can be a check.
Then running nonlinear, the solver verifies that:
- if VM >specified yield. plastic strain occurs
- if not, elastic range
The criterion does not verify the components. That means that any of components may be larger than the Von Mises. But the nonlinear only verifies VM
This is not an issue from FEM. It is material behavior.
Most metals exhibit Von Mises as plasticity cirterion. Then you have isotropic/ kinematic. And for other materials: drucker –prager, …. where the plasticity criterion is other.
If you read the Nastran help
NX Nastran supports the following types of yield criteria:
When I change the material type fom Plastic to Nlelast, I do not have the problem with the component stresses being greater than the last value on the strain-stress curve>
But in this case you will not have plastic strains. The material behaviour is different.
- non linear elastic: I do not remember but I think there is not plastic strain but the relationship stress/strain is non linear. In fact when you swicth to this option, you are not allowed to choose yield criterion
- the elasto-plastic/plastic or plastic you choose the yield criterion. If you are with steels Von Mises should be the right one. When the material reaches VM then the solver says: ok plastic strain occurs.
I am a bit lost sorry. First I would run linear. Check that VM is the same in any coordinate system (should be). Then I would go to non linear. Then choose VM cirteion if you are with "normal" steel and then check plastic strains, etc.
When you say "the solver says: ok plastic strain occurs", what do you realy mean? I stick to my initial question: why I get stresses bigger that the last value on the stress-strain curve? I was expecting this willnever happen!? Where am I mistaking?
the procedure it is like this (in a few words):
- solver calculates the stress components
- according to the criterion, let's say VM, calculates Von Mises
- VM>yield that you specify. Plastic strain occurs .It enters in the stress-strain curves
So imagine you have these stress components and yield of 400:
xx=100 yy=200 zz=500 xy=0 xz=0 yz=0
VM is 360MPa (It was a quick calculation). Stress components (zz)are larger than yield (VM) . You said stress components larger. But VM is not larger than 400. So in this case you have stress componenst larger that the last value of your curve. But VM is lower than yiled so no plastic strain occurs
I hope this helps. If not , some screenshoots of results may help