Cosmos Tube pull test vs actual test 1

[CR100]

While using cosmos we did a comparison of simulated load in cosmos and then an actual pull style loadtest. The results were vastly different.

The material in question is 1 3/8 dimaeter DOM tube with a 5/16" wall thickness. The actual material has a tensile of 60KSI with a yeild of 50ksi.

The application basically pulls on each side of the tube with a force of 25000lbs. This effectively stretches the tube. You can see from the picture there is a slight bend in the tube.

Cosmos correctly identifies the stress location, but when comparing the factor of safety cosmos produces 0.22. Which indicated that cosmos predicts the tube can only handle a load of .22 x 25000lbs. Maximum stress was 231447 psi.

When having the tube pull tested, the real world test we showed the bar still holding strong at over 49000lbs with out any major deformation.

Am I doing something qrong in cosmos? The setup if faily basic I select the material, create a restraint (normal to face) on one end of the bar. The create the force (normal to face) on the other end of the bar.

 

[DFLewis]

Are you using a linear or non-linear stress analysis?

An initial thought that came to mind is your material is being represented as a linear approximation of the actual properties of the material. For a linear stress analysis, any stress or strain data observed past the yield strength of the material will NOT be accurate.

On the other hand, a non-linear stress analysis will generally use actual data points from tested materials (one FEA program we use can pull data from Matweb.com). This will give a better result for the behavior of the material past its yield strength.

Your actual pipe will exhibit stress-strain phenomena that are not represented in a linear stress analysis alone.


DFLewis

http://www.phoenix-engineer.com

 

[rstupplebeen]

1. Is non-linear geometry on?
2. The end with the load should probably be constrained to only move along the axis of the tube as if it were in a rigid load frame.
I hope this helps.

Rob Stupplebeen

 

[gfbotha]

Material linear vs NL?
Geometrical NL?
Mesh refinement?
Hand/manual calcs?

You have a very large influence on the answers Cosmos spits out! What is the purpose of this all?

 

[kellnerp]

Cosmos correctly identifies the stress location, but when comparing the factor of safety cosmos produces 0.22. Which indicated that cosmos predicts the tube can only handle a load of .22 x 25000lbs. Maximum stress was 231447 psi.

What do you mean by this?

You need to tell us a whole lot more about the model.

[ol i]
[li]Solid or shell elements?[/li]
[li]If Solid, how many elements through the thickness?[/li]
[li]Was this a linear or non-linear analysis?[/li]
[li]If non-linear, did you use non-linear elastic, kinematic hardening or isotropic hardening?[/li]
[li]Was geometric non-linearity turned on?[/li]
[li]What is SW computing the FOS for? Yield, Ultimate, buckling?[/li]
[li]Where did you get the material properties for the tube? Ryerson or a similar handbook or did you send the material to a lab for a proper tensile test?[/li]
[li]Did you measure deflection and compare that at different loadings to see when the disagreement started?[/li]
[/ol]


Also, please don't use a picture posting service that has links to porn. Eng-tips has a quite satisfactory service at engineering.com.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[EdDanzer]

If I’m not mistaken tensile and yield strengths are not used in calculating stress or deflection in Cosmos. Poisson’s ratio is more important and correct values for a specific material more difficult to obtain. DOM tube is cold worked and should have different material values than standard library materials.

You should compare deflection results between Cosmos and your test to further refine your methodologies.

Ed Danzer

http://www.danzcoinc.com

http://www.dehyds.com

 

[gfbotha]

Actually a very good tutorial / sample problem in basic FEA because it touches on quite a few aspects!

Ed, I have found that often guys are not aware of the increased strength caused by drawing.

 

[kellnerp]

You only get the increase in yield strength after first exceeding yield and this is material dependent as well. This is not the case here except in the sense that the DOM process cold works the material. However, if he is using material properties for the tube at hand that is already factored in.

I have seen mass produced axles get 100+ksi yield out of 1008 steel due to massive plastic cold working. These properties were highly localized in the part and required extremely tight quality control to be viable.


TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[CR100]

Thanks for all the replies, I will try to add more info.

I am using static linear analysis mode. I have updated and constrained the one face to prevent any other movement then axial. This made a small improvement to FOS .36 from .26.

The model is test using a solid mesh. I'm not sure how to tell how many elements are used.

I have update the material properties using the manufacturers spec's.

 

[kellnerp]

OK, I see a big problem here. You are comparing a test case in which you undoubtedly caused plastic deformation to an FEA calculation in which a) geometric effects were not accounted for and b) in which yield was the failure criterion.

How did you determine when the tube began to yield in the test? That is the load at which you should compare a static elastic analysis to the FEA. Did you strain gauge the test article?

Can you tell us that the test article resumed it's original length when the load was removed?

If your FOS went from .36 to .26 it is getting worse since you want something greater than 1.0.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[BlasMolero]

Dear CR100,
Well, this is a general problem I see in beginners FEA users, trying to compare real life data test results with FE results. In general is a disaster, not agreement at all, because real life is really complex despite it seems very simple. In fact, to fairly compare compare virtual & test data results you will have to create an accurate FE model, that means many things & factors to have in mind: type of mesh approach (meshing the tube with 1-D beam elements, 2-D Shell elements or 3-D massive solid elements, and here the horrible TETRA10 is a disaster if you want accuracy, better solid brick HEX8 elements, or better 20-nide u/p brick elements and the best using 27-node u/p brick elements, you must solve the problem using ALL type of elements to compare results), second the mesh density (minimun two elements in the thickness), also very important how you apply loads & define constraints, of course to use an elasto-plastic nonlinar material model used, and of course to perform a nonlinear static analysis with loading/unloading + large displacements ON to account for stress stiffening geometric efects, and solve the model using an incremental & iterative solution process. At the end you will have accurate FE data results to compare with data test results, and if all assumptions are done OK the results will fully agree.

But if you mesh with tetra4 (draft) elements, with only one element in the tube thickness, perform a linear static analysis, etc.. then the FE simulation will not agree at all with real life.

Best regards,
Blas.

 

[TheTick]

I just did a pull test to determine the spring constant of an odd-shaped structural member. The results were scary.

The reason was that COSMOS allowed the mamber to flex sideways as it stretched. I had to constrain each end as if it was being stretched along a rail. Then the results corresponded with the hand calcs and actual observations.