Contact analysis between rigid and deformable problem 4

[Janus3]

Hello, I am a newbie to ABQ, so please have patience with me .
I am modeling contact analysis between rigid and deformable (elasto-plastic steel) body. The problem is axisymetric, the rigid body is wire. The interface is free interface (I used tangential frictionless behavior). When applying load, after certain amount of deformation the deformable body enters the rigid one- which is, obviously, bad analysis. I have tried to use smaller time increment and much finer mesh on the contact surfaces, but none of this seems working. Can any of you advise me what to do?

 

[Janus3]

I forgot to add some details of the analysis, I am using ABQ 6.4, the contact is established in Initial step before applying load, the load used is actually displacement. The elements are axisymmetric 8 nodded hexahedral elements. I realy hope someone can help me.
Thank you in advance.

 

[psantunes]

Hi janus!!

Please tell me if the deformable boldy penetrates the rigid body near the revolution axis?

psantunes

 

[harry123456]

Hi,
There is a similar problem of a rigid cylinder contacting a foam surface in manual. Take a look at that. Try using a small amount of friction. In some problems that I have done, it converged better with friction!!. Also maybe start with just the elastic material first and see if it converges and then go to the elastic plastic one. Also look at the message file (file.msg). Is it not converging because of contact (look at severe discontinuty iteration messages) or because of equilibrium not being achieved? Does it abort early on or later in the analysis?
Harry

 

[Janus3]

Hi, thank you all for the answers.
2psantunes: Yes, the deformable body penetrates the rigit near the revolution axis but it might be as well misleading as there really is a highest deformation in the direction of rigid body.
2harry123456: I will try and I will get back here.

 

[Janus3]

2harry 123456: the analysis does not abort at all, it completes successfully, the results are what worries me as they are not realistic.
The elastic material with little friction is better but after larger deformation (comparing to elasto-plastic one) it penetrates again. When using elasto-plastic material with little friction it behaves similarly as described above...
I have looked at the indentation of elastomeric foam with a rigid punch and when I have increased the amount of indentation, the foam also penetrated the punch during the analysis.
Do you think it is a failure of material or failure of analysis or maybe bad material model...
I can not explain, which bothers me a lot.
Thank you again for your kind advices.

 

[psantunes]

Hi Janus!

Try to do the following:

Impose Boundary conditions in the nodes placed at the revolution axis of your deformable body (use the edge selection option). If you are imposing the displacement in the direction U3, define U2=U1=0 at that nodes.

Psantunes

 

[bassmanjax]

If you are carrying out an axisymmetric analysis, how can you be using hexahedral elements? Structural axisymmetric analyses are 2D with DOF in 1,2 and 6 (rotation about the 3 axis).

As psantunes says, you will still need to impose boundary conditions to any nodes on the axis of symmetry (U1=0)

Also, have you got NLGEOM set in the *STEP option?

Martin

 

[harry123456]

True, You should have NLGEOM. I dont know if this will help as much because a rigid body simplifies the analysis-- you might want to try doing the analysis with a deformable body in pkace of the rigid body but put the stiffness of the body really high.
harry

 

[Janus3]

Thank you all for your kind advices.
the elements are CAX4R - axisymetric stress elements. I am imposing displacement in the U1 direction , the nodes on the revolution axis are fixed in U1 and UR3 direction, can freely move along the axis of symetry. Still experiencing the same problem, after certain amount of deformation and when the Deformation scale factor is set to 1 the deformable body penetrates into rigid one.
Finally I have used the NLGEOM and it works!!! Thank you very much for cooperation I hope this discussion could save someoene elses time as well.