contact convergence issue

[harry123456]

Hello,
I have gone through the archives and read as much as I can on dealing with contact problems. But I am still getting some problems. I have a 3D riveting analysis with two aluminum plates. the plates have a soft adhesive material in between and the rivet joins these together. large deformation and plasticity and contact.
I am using Standard and have run the problem till 85% of the time step. Using *Static,Stabilize and Automatic Tolerances helped. But after this time period abaqus cannot resolve the contact and keeps going through severe discontinuity iterations (closures and openings) cuts back and finally aborts.
I have gone through the manual but I am not clear exactly how I can overcome this. Refining the mesh would help? but I have a limit to which I can refine it. Any advice would be great.
Thanks
harry

 

[Drej]

Harry

Have you checked the deformed shape of the model prior to failure to see what's happening? Is the error due to some type of limit being exceeded (material, rigid body motion, etc.). Is the contact becoming separated? What type of contact do you have? Have you tried reduced the initial time step? Have you tried applying the contact (to "just touching") in one step and then applying the pretension in the rivet in subsequent steps (if that's how the analysis works)?

Cheers,

-- drej --

 

[harry123456]

Hi
I have normal Master Slave contact. In the rivet and adhesive interaction the adhesive is the slave (its elastic but very low stiffness). I have refined the slave more than the master.
I have tried reducing the time step as well as applying load in subsequent steps.
I have contact between the adhesive and the rivet as No separation after contact. Maybe thats making a difference? From postprocessing It seems there are a few elements that are deforming and leading to contact issues ( i apologise but its kind of difficult to describe)
basically the error is that abaqus goes through the contact
severe discontinuity iterations: 1 closures 0 openings etc
and keeps on cutting back on increments and dying out.
any suggestions? I will try some more things and post more info
harry

 

[Drej]

How are you modelling the plates/rivets/adhesive? Is it a 3D solid model? Does the adhesive have peculiar properties (hyperelastic, for instance). Is some perturbation level being exceeded (localised collapse somewhere say?). You may want to switch linesearch on (if it isn't on anyway) as well - with the presence of contact, linesearch is usually switched on by default in most FE codes. In some instances linesearch can speed up the solution considerably and work for you (plasticity and contact especially). If your analysis is load controlled, you may have to switch arclength on also to get over any perturbation points.

I would guess that your contact is probably causing you the difficulties, but it's difficult to say. Can you apply a fully bonded condition for all your components throughout the analysis as a a starting point? From there it may be easier to debug. If that runs ok and looks sensible you could try with a more exotic type of contact (frictional, say) and build your way up. If anything, you'll know exactly how your model is performing by carrying out these small benchmark cases. Without the details of your geometry/loads/etc. it's really difficult to say exactly what the smoking gun could be.

Cheers,

-- drej --

 

[harry123456]

Hi Drej,
The model is 3-D solid meshed with C3D8R. Initially I was using a hyperelastic material for the sealant in between the plates but that was hard to resolve so I started with this initial model by modeling the sealant as linear elastic but very low stiffness (0.1e6 psi) in comparison with the aluminum plates (10e6 psi) (basically properties of an adhesive). Right now I have frictionless contact for the adhesive and plates. I have linsearch on. I have displacement applied as the load (thats the data I have) I am carrying out benchmark cases by trying out the control and contact control parameters to see how it affects the analysis.
When you say bond do you mean TIE the surfaces together?
thanks
harry

 

[corus]

You might have a problem with 'chattering' where a single node opens and closes. Look at the surfaces to see if one node is falling off the edge of the other surface. You can also modify some parameters in the contact controls definition so that a single opening or closure is allowed for convergence. If you have too much non-linearity in the problem you might have more success using explicit rather than standard.

corus

 

[harry123456]

Hello,
I am still working on contact convergence of my model. I just had a quick question that I didnt understand from the manual. When you define the normal behavior as "Exponential" contact, how do you enter the value of pressure for the clearance?
When you use *Contact Controls, Approach. What exactly is that?
sincerely
harry

 

[corus]

I have no idea about the exponential approach as I tend to use 'hard' contact.

Contact controls gives some contol over the iteration process. Using automatic tolerances does help the solution but you can always try modifying the other parameters. MAXCHP should stop chattering problems at a single node but for some reason it didn't seem to work for me.

corus

 

[Tamlin]

Hello harry,

the contact definition with

*SURFACE BEHAVIOR,PRESSURE-OVERCLOSURE=EXPONENTIAL
clearance at zero pressure
pressure at zero clearance

is a soft contact definition. It's fine when you
have this "chattering" of nodes corus mentioned.

Hope this helps.

Tamlin