Tensile Test Validation

Altair Forum User

Hello all,

I was recently messing with the tutorials in the non linear analysis chapter and this post references to the TUTORIAL: RD-3500.

For better understanding, here is a quick resume: It is about a non linear simulation of a tensile test plate with anisentropic material property. It is modeled as PShell with a Thickness of 1.7mm. So far so good.

Now here comes the part where it gets strange. The tutorial says: You can model this tensile test with only a quarter of the elements. So I went on and did that analysis and all went well. I was asking myself at the end of the test: What if I want to model this in Solidthinking, would it not be better to run it with all the elements. So I translated the elements (duplicate, reflect) and equivilanced it. I set the boundary conditions as I would expect it to be in a tensile test machine. One end I was holding with all DOFs fixed, the other was moving with the given velocity. It looks like this in my model:

I then went on and ran the simulation: It did not break.... and that I can not explain. If it is correct to calculate my simulation with only a quarter, it should be the same if done with all the elements. I then went on and checked if my model breaks at all, and that concludes in:

Quarter: T=10s Break

Full: T=15s Break

The only thing different are the boundary conditions. But I can not see my mistake. Hope you guys know any solution for that.
I was running it all on HW11. I am getting HW12 soon but any tips on how to easily get an animated version of my result file in Solidthinking would be great. Did some experiments with it but keeps crashing on lager *.h3d files.

Have a nice weekend.

Merula

Altair Forum User

Merula,

The difference in results should very clearly be due to the change in the boundary conditions,

How are you scaling the boundary conditions to the full model? the full model should have the same proportional boundary conditions as the quarter model. This is not simply scaled.

Altair Forum User

Thanks Rahul,

ok then let me reformulate the problem: I do not want to check the scalability of the solver but if the simplifications I made at the breaking point were correct.

As a conclusion I would suppose they were not based on different results.

Is this conclusion proper?

Altair Forum User

merula,

This is not about the scalability of the solver, it is the scaling of the model.

The imposed velocity should change from the quarter model to the full model, correct? A bigger model with the same imposed velocity will give different results , when you are scaling the model (making it bigger) the boundary conditions must change as well.

Altair Forum User

As the HyperWorks Student guide says - Practical Aspects of Finite Element Simulation A Student Guide

'Symmetric conditions could be used only when both the following conditions are fulfilled.
1) Geometry is symmetric
2) Boundary conditions (forces and constraints) are symmetric.'

Since you are going for a full model from a quarter model the same rules apply,

'Symmetry can greatly simplify a problem by reducing its size and complexity both during the
solution and preparation phases. Care must be taken however to ensure a consistent set of
symmetry boundary conditions. In order to use symmetry assumptions both the loads and
boundary conditions and the actual geometry must be symmetric.'

read about symmetry boundary conditions in chapter 10 and in other areas of the guide.

Altair Forum User

hanks again Rahul for the reply. It is just that I did not scale the model at all.

In the tutorial it is about a tensile test model which was reduced to a quarter (but not scaled). I then thought I want to test if the full model (not only the quarter model) would work the same.

The Constraints at the breaking point are used to simplificate the model from full to 1/4. These I can not have in the full model because it makes no sense to do so.

Is it the size of my model which causes the difference in the breaking point time?

Altair Forum User

merula,

Please recheck for I get exact one to one similarity of results between the quarter model and the full model at the relevant times, i must investigate the breaking time,
how are you estimating the break time?

I have attached my model for you to investigate (tensile_full)(please rename to rad to solve, please remove both option while solving as I have merged solver and engine file). please change output tstop to a higher value.

With my previous comments I was trying to state that the boundary conditions must be different for different models especially in case of symmetry where smaller model is being scaled to full model.

So I see from your image that you do change the velocity constraint to be applied to the whole of the left end of the model

I also see that you have changed the constraint boundary conditions to be applied to the whole of the right hand side of the model.

The constraint however does not seem to be the same as in the quarter model, it looks in the image that you constrained all the dof, did you try to constrain with just Tx, Ry and Rz as in the quarter model? what other changes are you doing to your model?

,

Altair Forum User

Rahul,

thanks for that detailed answer and for the solving deck. I think it is best if you see my quarter model analysis and your full model analysis in comparision for the full time. I uploaded an .avi video which I renamed as .jpg.

In the video you can clearly see that the vanMises Stresses differ and that there is some contraction on the quarter model at the breaking point zone which is typical for tensile tests. I do not see those contractions on the full model which is the first thing. The second thing is that at the end of the animation you can see a rapid decrease of the van Mises stresses on the Quarter Model. This to me indicates a break.

In this case quarter model and full model differ and I do not know the reason why it is like that.

Altair Forum User

merula,

I see now that I had not entered the plasticity hardening exponent value (n in the material), with this change the test specimen fractures as expected. Please do this change in the model I sent earlier, recheck and reply.

Altair Forum User

I have attached the full model here which will fracture as expected, Please check at your end and we can discuss further

Altair Forum User

Thanks Rahul,

yes indeed the tensile test breakes now in the exact same manner as the quarter model but at different times. Where I see the quarter Model break at T= 9 seconds, the full model breaks at T=15s.

Where comes the difference from?

Altair Forum User

merula,

The full model clearly fractures at 15 seconds, when you see the 0001 out file you see that the rupture is recorded,

RUPTURE OF SHELL ELEMENT NUMBER

Interestingly a very similar result of 15 seconds rupture is seen in a half model as well, I strongly recommend you try the half model for interesting results 

You need to recalculate the fracture time/criteria for the quarter model, The tutorial says nothing about the fracture time, just that the simulation is run for 10 seconds, maybe they were just interested in the necking of the specimen?

So once your fracture/rupture time estimate of the quarter model is more clear we will discuss further 

Altair Forum User

I have now the answer: As we doubled the stiffness by doubling the elements we had to double the force, which I did not. So Long terms short:

Force follows model size!

Altair Forum User

That is great news 

This is just as I suggested in the very first post, the boundary conditions (force here) must be proportional to the model

Altair Forum User

hi prakash, 

 

how to get fracture in result.

Altair Forum User

Hi,

 

You can model fracture using

 

1. A damage model in Law 27

 

2. Failure using the Johnson-Cook model

 

3. Forming Limit Diagram as a failure model

 

4. XFEM method for crack propagation

Altair Forum User

thank you

Altair Forum User

Is it possible to performe composite material tensile test with fractures result?
If possible, 

what are steps i have to follow?

Thanks for your support

Altair Forum User

Hi,

 

Please contact your local support.

 

Commercial customers can take advantage of hotline support. 

 

If you are commercial customer, please contact your local support.you can contact your local support @ http://www.altairhyp...ortProduct.aspx

Altair Forum User

Thanks for your sharing. Textile Tensile Testing Machine is designed to test a wide range of materials in tension, compression, flexure, shear, and peel. Textile Tensile Strength Tester complies with ISO 13934.1/2, ISO 13935.1/2, ISO 9073.3/4, etc. It might provide you with some help, please click on https://www.testextextile.com/product/textile-tensile-testing-machine-tf002/