Sequentially Coupled Analysis

[ysg519]

I am simulating a sequentially coupled thermal analysis. I am working with an assembly. I have completed a thermal analysis and then modified the input file for element type, predefined field, boundary conditions(after saving under a different name). I keep getting an error that "abaqus exited with error" with no other explanation in the log file. There is no message file generated.
Could you please look at part of the input file below and see if something is grossly wrong.
Some more info
1. I used tet mesh in thermal analysis with DC3D4 elements
2. In the following mechanical analysis I kept the same mesh and changed the element type to C3D4
3. Used .odb file for predefined field temperature data.



** INTERACTIONS
**
** Interaction: moly-part3
*Contact Pair, interaction=IntProp-1
cebaf_asm-3-1.side, molymn-1.insdang-lft
** Interaction: part1-moly
*Contact Pair, interaction=IntProp-1
molymn-1.outsdsd, cebaf_asm-1-1.side
** Interaction: part2-1
*Contact Pair, interaction=IntProp-1
cebaf_asm-1-1.outrbtm, cebaf_asm-2-1.btm
** ------------
**
**
** STEP: Step-1
**
*Step, name=Step-1
*Static
1., 1., 1e-05, 1.
**
** BOUNDARY CONDITIONS
**
** Name: BC-1 Type: Displacement/Rotation
*Boundary
_PickedSet18, 1, 1
_PickedSet18, 2, 2
_PickedSet18, 3, 3
_PickedSet18, 4, 4
_PickedSet18, 5, 5
_PickedSet18, 6, 6
**
** PREDEFINED FIELDS
**
** Name: Predefined Field-1 Type: Temperature
*Temperature, file=cebaf_01convc.odb
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-1
**
*Output, field, variable=PRESELECT
**
** HISTORY OUTPUT: H-Output-1
**
*Output, history, variable=PRESELECT
*End Step

 

[ysg519]

Initially the model would not give me any details of error except "Abaqus exited with error". But when I deleted the boundary conditions I get this error.

***NOTE: SEVERE CONTACT OVERCLOSURES EXIST. CONVERGENCE IS JUDGED UNLIKELY.

I think the model which is an assembly of 4 parts has issues with contact. I have defined surface-to-surface contact in thermal analysis and it seems to be going smooth and gave me good results. But when I do the subsequent structural analysis as part of the sequentially coupled analysis I get the above overclosures error.

Any ideas how to overcome this problem. Thanks

Yousuf

 

[mizzjoey]

Hmm... could you see if there's any error printed in the dat file?

Regards,
jo

 

[corus]

As mizzjoey says, if there's no msg file then the error message will be in the dat file. I would point out though that it'd be a mistake to use C3D4 elements in a structural analysis and your results would be pretty much useless. I think you can convert your temperatures to fit a model with C3D10M elements (quadratic) though by interpolating the results for mid-side nodes.

corus

 

[ysg519]

Right now I am trying to simplify the model and do only a static analysis of the assembly. In the message file I get this error

***WARNING: SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING NODE CEBAF_ASM-3-1.166 D.O.F. 1 RATIO = 2.71455E+13.

I have tried a few options in the interactions but they didnt work. Please help. Thanks

 

[corus]

The error is in dof 1. Check your restraints in that direction.

corus

 

[ysg519]

Corus, as per your advice I will use C3D10M for stress/displacement elements and DC3D10 for thermal analysis. Right now since I think there are problems with overclosures I am trying to get the structural analysis part right by applying simple pressure load.

I have constrained a surface in all DOF as my boundary condition. However I did not see a blank against the 6 DOFs in which I could fill out zero to show full constraint. I have seen this earlier that gainst each DOF there is a blank box but in this case I did not see any. Would you know why this option is not available? Thanks.

 

[corus]

The boxes will be greyed out because you're looking at the initial step and not step 1. In the initial step you can only apply zero(full) constraints and hence it's greyed out. If you have overclosure then try applying fixed dispalcemnts as load case 1 to establish contact, then remove that fixed displacement in step 2 and apply your real loads. You'll have problems with quadratic elements in contact though and it's always best to try and mesh your assembly with linear elements and have a structured mesh.

corus

 

[ysg519]

Thanks Corus,
Yesterday I changed the step to initial and it worked and your message confirms it.
I continue to get negative eigen value errors. Is contact a problem even with linear tetra elements like C3D4? My model is a little complex I tried meshing with hex elements but partitioning the model was impossible. Any idea as to how to mesh such models with hex elements? I know hypermesh and other such software can mesh such models easily but I would like to know if there is a work around with in abaqus. Thanks again.

 

[mizzjoey]

If you have problems meshing with Abaqus perhaps you can do it first in Hypermesh and then export the geometry into Abaqus as an orphan mesh? Yes, 3D meshing with Abq is a pain sometimes. Using Hypermesh is a way to go around this but the problem with importing an already meshed part into Abq is that we can't edit the orphan mesh. At least, I haven't found a way to do it.

If you still want to mesh with Abq perhaps you want to check if your geometry needs to be repaired.

hope this helps,
jo

 

[ysg519]

mizzjoey,
Thanks for your suggestion. Unfortunately I don't have access to Hypermesh so I guess I am stuck with Abaqus

 

[corus]

In general you can mesh any geometry with hex elements, given time. Generally I've avoided hex meshing if it's a region I'm not particualrly interested in and the geometry is too complex to take the time partitining it down. To get a hex mesh you need to have an initial strategy of how you're goign to break down the geometry. Without seeing the geometry then it's impossible to advise. There is an attachment feature here where you can upload a file. Try uploading a picture of the geometry.

If it's a complex problem you have with contact then it's better to try and simplify it first and then build in the complexity later to see how far you can go. I know if you bang in plasticity with large displacemnt and contact between several objects then there's fat chance of it working straightaway.

corus