Question in linear and nonlinear analysis
Question in linear and nonlinear analysis
(OP)
I am using Ansys 7.0 to do a FEA on a torispherical head subjecting to internal pressure. According to my understanding, I should triger a nonlinear (material) analysis, especially at a thinner head thickness. I started at a thicker head thickness which limit the stress-strain relationship in the linear elastic zone on the stress-strain curve (engineering). I tried linear model (E=27.5 ksi) and nonlinear model (which has the same E=27.5 ksi for the linear region, and use several pionts to simulate the plastics zone). What I got is the different results from different models EVEN THOUGH the stress-strain relationship is in the linear zone. This really confused me! With the same E=27.5 ksi in linear zone of both models, why did I get different stress and strain values? The result from nonlinear model is considerable lower than that of linear model. For example:
for the same area as I am interested:
Linear model: strain range - 0.0007 to 0.001 stress: 19,000psi to 27,000psi
Nonlinear model: strain range - 0.0005 to 0.0007 stress: 13,000psi to 18,000psi
I have exact the same model setup for both models (meshing, boundary conditions,......).
The results fit the stress-strain cuver very well for both models. My question is why the results are quite different from different models with same E-27.5ksi in the linear elastic zone? I have checked that both models are using the same solver - Sparse Direct Solver.
Thank you for the help in advance!
Yi
for the same area as I am interested:
Linear model: strain range - 0.0007 to 0.001 stress: 19,000psi to 27,000psi
Nonlinear model: strain range - 0.0005 to 0.0007 stress: 13,000psi to 18,000psi
I have exact the same model setup for both models (meshing, boundary conditions,......).
The results fit the stress-strain cuver very well for both models. My question is why the results are quite different from different models with same E-27.5ksi in the linear elastic zone? I have checked that both models are using the same solver - Sparse Direct Solver.
Thank you for the help in advance!
Yi





RE: Question in linear and nonlinear analysis
If this is how u input data and your yield point is about 13000 psi then your results make sense, otherwise check ur stress strain data points.
fsi
RE: Question in linear and nonlinear analysis
The material is 304 S.S. My first point is the point where the material shows deviation from the linear slope (E=27.5ksi). The point is appoximate at strain=0.00095 and stress=26,100 psi. When the strain-stress range is in the linear elastic zone, why did I get the quite different result from different models? Here are the points I input:
Strain Stress
0 0
0.00095 26,100
0.0013 31,900
0.0018 37,700
0.0025 43,500
0.0032 46,400
0.0048 49,300
The E for the first section of the input is 26,100/0.00095=27.47ksi, I think it is very close to the 27.5ksi,right?
it is obvious that the results from both models are in the first section of the input: 0 - 0.00095 / 0 - 26,1000. So I think I should get the same result for the interested area by using any model, but it is not. Of course, when the stress-strain moves into the following zones, the E is becoming smaller and smaller since it enters the plastic zone. But for the first zone, the E in nonlinear model is the same as that in linear model, the result should be the same if the calculated stress and strain are in this zone.
RE: Question in linear and nonlinear analysis
fsi
RE: Question in linear and nonlinear analysis
That's my 2 cents, because I spent months troubleshooting these very same type of problems with FEMAP & Nastran.
tg
RE: Question in linear and nonlinear analysis
For thin walled pressure vessels, you should be running a non-linear analysis because deflections of the shell typically are very large in relation to the thickness. The geometric non-linearity will consider membrane tension effect in the shell, which, like a balloon, will help with load carrying of an internal pressure. As the vessel deflects under incrementally increasing load (load steps), ANSYS will re-calculate the stiffness matrix considering membrane tension and also the change in inclination of applied forces (i.e. follower forces).
Long story short... your results sound correct to me.
RE: Question in linear and nonlinear analysis
As I have not used ANSYS in awhile, I apologize if I am wrong. However, my recollection of ANSYS (and my experience with other codes) leads me to believe you have made a mistake in interpreting/inputting your stress-strain curve for the plastic model.
FEA programs operate on true stress/plastic strain for metal plasticity models, and this is usually reflected in how the programs expect their stress-strain data.
Normally, I would expect the first data pair to be a "0" for (plastic) strain, and the stress for first yield. In your case, this would be (0.0, 26,100). By inputting your first point at (0.0, 0.0), you have described a material which is effectively plastic immediately.
Again, I haven't used ANSYS in many years, so this may be an acceptable means of inputting a plastic curve. But this is not the "classical" means of inputting such data.
Hope this helps,
Brad
RE: Question in linear and nonlinear analysis
If Ansys is set up like IDEAS, then your first point should be (0.00095,26100) not (0.0,0.0), If you delete (0.0, 0.0) , I think you should get the correct results.
fsi
RE: Question in linear and nonlinear analysis
This is a wonderful forum with great people, I am really enjoyed!
Yi
RE: Question in linear and nonlinear analysis
corus
http://www.corusresearch.com
RE: Question in linear and nonlinear analysis
Just to clarify somethings here:
plasticity is material nonlinearity where as stress sitffening and large displacement are geometric nonlinearities.
fsi
RE: Question in linear and nonlinear analysis