Question in linear and nonlinear analysis 1

[proe2003]

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

 

[fsi]

what is the yield point of material? Your first point on the stress strain curve data should be the yield point.
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

 

[proe2003]

Thank you, fsi.

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.

 

[fsi]

I agree u should get the same results if your stresses and strains are in the elastic range. Check your setting for nonlinear model and check your load factor, time, etc. There is some setting that is kicking you into nonlinearity before it is time. Having said that strain of .001 and stress of 27000 psi is in the plastic range?
fsi

 

[trainguy]

You should contact ANSYS. Every code has specific details about how nonlinear materials should be defined, and this is sometimes not obvious in the reference manual.

That's my 2 cents, because I spent months troubleshooting these very same type of problems with FEMAP & Nastran.

tg

 

[scofie]

I may be off here, but I think what you are seeing in your results is the effect of geometric non-linearity, NOT material non-linearity. Perhaps the ANSYS solution you are running includes both types of non-linearity.

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.

 

[brad]

You state "here are the points I input..." and then describe (0.0,0.0), (0.00095,26100)...

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

 

[fsi]

proe2003
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

 

[proe2003]

First of all, thank you for all your guys to give me the help. Yes, the first input point is (0.00095,26,100) instead of (0,0). (0,0) is the default point in Ansys, which I believe. As Scofie pointed out, I considered the geometric nonlinearity in the linear model, then the results are just beautiful, really make sense. In the nonlinear model, I could not find the place to select "large displacement effect" and "stress stiffness". I believe that the program will do this automatically, which really make sense since plastic deformation will occur.

This is a wonderful forum with great people, I am really enjoyed!

Yi

 

[corus]

I would check the code again as large displacement does not automatically come with plasticity. If I remember well I also think that stress-stiffening is also an option you must choose in Ansys.

corus

http://www.corusresearch.com

 

[fsi]

proe2003
Just to clarify somethings here:
plasticity is material nonlinearity where as stress sitffening and large displacement are geometric nonlinearities.
fsi

 

[Drej]

Just a further note that stress stiffening effects default to SSTIF,ON when NLGEOM,ON (and SOLCONTROL,ON) is issued.