Too many attempts for Increment Error!! 3

[ConorWalsh]

hey all,

I am using the macro tool to record myself importing geometry and then setting up contact between parts automatically.

Then I change the 2d iges files I am importing using another cad package (catia) and am trying to get a contatc analysis to run with the specific geometry I have imported.

Anyway the problem I am having is that sometimes when I import the new gemetry and submit a job it works and other times I get the error 'too many attempts made for this increment error'

I am quite confused and hoping someone may know what this means

Thanks again

Conor

 

[corus]

Usually in contact you can get 'chattering' which causes it to continually iterate. See which node or nodes are opening and closing to see if this is the problem and then vary the contact parameters to see if that will stop it or use stabilize, or use linear elements which work better. I have no idea why the imported geometry should affect it.

corus

 

[ninguno]

i am very much a black box user of abaqus, but...

i found that when I had this problem, my (complex) surfaces weren't properly sticking together when using a tie.

I found that by upping the tolerance for the constraint, the number of unconstrained slave nodes dropped and the model appears to work as expected.

 

[kize]

Hi, Do you define contact in ABAQUS/standard?Try again with ABAQUS/explicit.

 

[labosonic]

As corus said, using a stabilize option can be a correct solution but take care using this option because it can also help convergence of an analysis by giving unphysical results.

The way of solving problems is to check all infos in your .msg file :
first by running an analysis with *PREPRINT,CONTACT=YES in the model part of your .inp (between *HEADING and the first STEP) and adding *CONTACT PRINT in each step.

your analysis will give you very big .dat and .msg files with full info about all the contacts in the model.

Then many options :
- you read the contact details and detect "chattering" : a second order node opens, closes, opens, etc ... through the increments. Then use a more appropriate element type (linear element or 2nd order modified element - for example C3D10M instead of a C3D10)
- if you see that nearly all your contacts are realized and few are still opened or closed, you can allow code to make more attempts in step by using the *CONTROLS card (be careful this area is full of parameters, check it twice before re-running analysis) the default must be about 5 attempts you can define a bit more
- if you noticed a large occurence of the word "overclosure" followed by tiny values (i-e 1E-7) AND if your loading/boundary condition is not too large, you can switch the automatic tolerances by *CONTACT CONTROLS, AUTOMATIC TOLERANCES in the step part. ((reset to *CONTACT CONTROLS, RESET) in the next step .

To limit the problems with contact always try to use displacement approach instead of FOrce approach if possible.