cancel
Showing results for 
Search instead for 
Did you mean: 

Define contact for stamping analysis

Creator
Creator

Hello everyone,

 

I have to simulate a bending analysis of a blade to determinate the residual stresses to be more accurate on an another analysis.

I saw an stamping analysis example and I try to replicate it for trianing.

Unfortunately, I only have acces to 101/106 solver so I can't manage both contact and plasticity but the goal is just to train.

 

Here is the example I try to replicate : 

assembly.png

 

I fixed the lower part and I force the displacement of the upper part.

 

I have some difficulties to define contact in this analysis, because there is different kinf of contact (surface contact mesh, surface to surface contact) and I don't understand well the difference between them.

 

I defined contact (with surface to surface contact) between upper part/ plate and lower part/ plate, and I have also used the "mesh mating condition". 

 

assembly load.png

And I have results like that : assembly result.png

 

The picture is not at scale 1.

 

So as you can see, I didn't set the contact correctly.

 

Can someone help me define contact correctly for this analysis ?

 

Thank You !

 

Arthus

7 REPLIES

Re: Define contact for stamping analysis

Creator
Creator

Hello,

 

I finally succeeded to set up contact correctly, but now I have a little problem to define the right boundary condition.

 

First, I did my analysis without any boundary condition on the plate, but no solution was calculated by the solver. So I tried to fix an edge and it worked but it does not match with reality because the plate is free to move during the stamping process.

Deformed ShapeDeformed Shape

So what boundary condition do I have to use to have a realistic solution ?

 

Thank You.

 

Arthus

Re: Define contact for stamping analysis

Valued Contributor
Valued Contributor

Dear Arthus,

 

This is a symmetrical problem, consequently you could add restraints to the centre of the plate. Done properly this should  not affect your results. Possibly you also need to add some weak springs if the solver still reports singularity. The springs could be connected to the "ground" or to the bottom part being restrained.

 

Please also note that you could model only a half of the problem and apply symmetrical boundary conditions. This would give you a much smaller model, signicantly reduced solution time and partly also solves your problem with the boundary condition/stability.

 

Best regards

Geir Olav

Re: Define contact for stamping analysis

Creator
Creator

Dear Geir,

 

Thank you for your answer.

 

I have now considered the symmetrical condition.

As you recommend it, I tried to add a spring connection between the plate and the fixed part.

I have used the "edge to edge connection"  on the left edge (ref to previous image) of the plate and I chose CBUSH1D connector. Is that what you meant by "weak spring" ?

Also I left the right edge free but it does not move during the stamping process, it's like the edge was set with a fixed constraint. Do you know why this happen ?

 

Best regards,

 

Arthus

Re: Define contact for stamping analysis

Valued Contributor
Valued Contributor

Dear Arthur,

 

My proposal is to use weak springs if the solver reports singularitites. It could be for instance three springs connected to different nodes and in different directions. I don't think you should use the edge to edge connections. With weak springs I mean springs being defined with so small stiffness that they don't have significance on the result, but give you the required stiffness for the solver. You could start with stiff springs and reduce the stiffness if you get results and observe that peak stresses are found at the spring connection points.

If your outer edge don't move I would expect that something is wrong in you model. 

 

Best regards,

Geir Olav

Re: Define contact for stamping analysis

Hello Arthus,

 

Lastly I tried to do similiar simulation. You can find some information about the contacts in here: CGap & CBush

 

With reference to the contact and solution:

To include the plasticity you can simulate the contact by use of CGap or CBush elements in SOL106, however this is reasonable for small displacements (I think so?). Here the displacements seems to be quite large with respect to the size of the model so it may be that the results may not realistic? For sure SOL106-601 (ADINA) is a better option in here. What's more, in stamping the friction is a quite important, so in SOL106 it will be probbably not possible to include all relevant phenomenas. Maybe anyone "who knows" can tell more about it.

 

With reference to the boundary condition, try to split the surface of your "bended" plate where you do not expect any lateral movements and fix it in few nodes/points. In your case it is a Z-axis. This should prevent agaist matrix singluarities. The springs that has been mentioned by Guddal: I think he meant a CElas (the most simple spring element). What is more, I can see that you defined contact only between the 'bended' plate and the upper 'stamp' only in the 'bulb region' (and additionally between the upper and lower stamp) but there is no contact between the plate and the stamps in the 'flat regions'. Consider whether your contact are in every region they should be (in general there should be contact 'all-to-all').

 

Wish you luck!

Re: Define contact for stamping analysis

Creator
Creator

Hello Tomek and thank you for your answer, it helped me !

 

Now I do my study directly on the piece I need, but it is quite similar to the previous study.

 

The goal here is to give a curved shape to the blade thank to the cylinder.

 

As you recommend, I set up CGAP elements (1D Connection -> Node-to-Node -> Proximity) between the cylinder and the blade without forgetting to set also the element orientation and properties.

I apply a pressure on the blade so that the load is always normal to the surface.

Here is what it looks like : 

config.png

But now, it seems the calculation never ends and oddly the load step starts a 1.0.

load step.png

Is that a convergence problem, or it is still a contact problem ?

 

About the element orientation, I'm not very sure how to define it correctly because here, the contact is between a curved shape and a flat shape so I chose a cylindrical CSYS type. Is that correct ?

 

Thank you ! 

 

Best regards.

Re: Define contact for stamping analysis

As I said before, I think that this case seems to be too complex for SOL106.However if you want, you can try, but the results will be not realistic. Remember that the orientation of the CGap Elements through the analysis will change dramatically, some of the elements will rotate about 90 degrees, so I think it's not correct.

With reference to the convergence: load you apply in a first step is too high. You should change the number of iterations in solution parameters. Try to run your model with the gravity only and probably it will converge (if model is stable).