ABAQUS/CAE JOB IS RUNNING SLOW 1

[BrendaGR99]

Hi guys,

Right now I'm running a coupled temp-disp analysis in ABAQUS/CAE, however, my job is very slow, 15 minutes have passed and only 1 increment has been made, I tried modifying the step to a time period of 1, maximum number of increments of 50, initial increment size 0.01, maximum 1 and minimum 1e-15. When I increase the maximum number of increments to a 1000 that seems to run faster but it may take days to finish. What can I do?

I attached my file if that helps.

 

[FEA way]

Check the warning messages printed when the solver is running. The model seems to be underconstrained. There's just one BC in the direction normal to the plate.

 

[NRP99]

Check "Spurious oscillations due to small time increments" in help manual. "In transient heat transfer analysis with second-order elements there is a relationship between the minimum usable time increment and the element size."

Some observations
-1W/mm^3 heat flux defined.
-Check units of material data. Unit of density for INVAR 36 seems wrong.

 

[BrendaGR99]

The warning messages are:
For contact pair (assembly__pickedsurf14-assembly__pickedsurf13), not all the nodes that have been adjusted were printed. Specify *preprint,contact=yes for complete printout.

Surface interaction intprop-1, associated with one or more contact pairs with surfaces having underlying elements with temperature and displacement degrees of freedom, does not have any thermal interaction defined. No thermal interaction will occur.

Where is the heat flux defined? Should I change it?

Concerning the units of the INVAR 36, I got the density from this link

https://f.hubspotusercontent20.net/hubfs/7407324/Material Saftey Data Sheets/Invar 36.pdf

Since my model is in mm I converted the .291 lb/in3 to tonne/mm3, I got 8.05e-6 tonne/mm3

 

[FEA way]

There should be also some warnings associated with singularities (underconstraint). They appear later on during solving.

Do you use parallelization (multiple CPUs) for this analysis ?

Heat flux is your thermal load. Just make sure that the value is correct. Units in thermal analyses can be really tricky.

It should be 8.05e-9 after conversion.

 

[BrendaGR99]

The job is still running, it's been going for 3 hours, there's 16 increments so far and there are no further warnings.

I didn't use parallelization.

I don't remember adding heat flux, I added an initial temperature of 20 Celsius.

Thanks for telling me, I will change the density.

 

[FEA way]

Apart from the initial temperature, there is a body heat flux load with a unit magnitude in your file. Maybe that's what causes problems, remove it if you haven't defined it intentionally.

Also, enable parallelization in job settings and specify the number of CPUs that your machine has. It will run much faster then.

 

[BrendaGR99]

After enabling parallelization and changing the density the job ran much faster but the job aborted at the 50th increment, which was my maximum, should I increase the maximum number of increments? The only warnings I got were the warnings that I already talked about.

 

[NRP99]

If there is no any other error that is related to convergence, you need to definitely increase the maximum increments as analysis requires more increments to complete. You can use 1000 increments as maximum increments if you not sure about how much is required.

Please refrain from double posting. You can use this post to ask more questions related to this (same) post in the same post.

 

[BrendaGR99]

For the heat flux I just realized that I did add one. I'm trying to mimick an autoclave process. For this I needed the model to pass through different temperatures at different times, to achieve this I added an amplitude, with the time being in seconds and the amplitude representing the temperature in celsius. Is this correct?

Here is the image of the amplitude.

 

[FEA way]

Yes, you can do it this way. Just remember to specify a magnitude of 1 for the BC or load using this amplitude and to stick with Celsius units for the rest of the analysis setup.

 

[BrendaGR99]

My job aborted after 207 increments, the error messages were:

Time increment required is less than the minimum specified

The analysis has been terminated due to previous errors. All output requests have been written for the last converged increment.

The warnings were:

For contact pair (assembly__pickedsurf14-assembly__pickedsurf13), not all the nodes that have been adjusted were printed. Specify *preprint,contact=yes for complete printout.

Surface interaction intprop-1, associated with one or more contact pairs with surfaces having underlying elements with temperature and displacement degrees of freedom, does not have any thermal interaction defined. No thermal interaction will occur.

In the message file, the following warnings were present:

***WARNING: THE SYSTEM MATRIX HAS 3 NEGATIVE EIGENVALUES.
EXPLANATIONS ARE SUGGESTED AFTER THE FIRST OCCURRENCE OF THIS MESSAGE.


***WARNING: SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING NODE
COMPOSITE-1.27 D.O.F. 1 RATIO = 32.7548E+09 .


***WARNING: SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING NODE
COMPOSITE-1.27 D.O.F. 2 RATIO = 33.0342E+09 .

My minimum time increment is 1e-15 so I don't think the problem is there, it is already pretty low. What can I do?

 

[FEA way]

How far did it go in step time ?

Those are the singularities I’ve mentioned before. Have you changed the boundary condition to eliminate rigid body motions ?

 

[BrendaGR99]

No, how do I eliminate that? Right now the only BC that I have is a Displacement/Rotation with U3=0 in the bottom face of the larger body. In step time it went till 0.000155 on the last increment.

 

[FEA way]

Try with also U1 and U2 fixed for this face. If it doesn’t help, replace contact with tie constraint. If it still doesn’t work, we will know that the problem is not caused by an underconstraint. Then the thermal aspects will be the likely cause.

 

[BrendaGR99]

With the U1 and U2 fixed, the singularities disappear but I notice that the top surface moves away from the bottom, I don't know if it's a problem with the contact. I tried ticking the "tie ajusted surfaces" box but that creates excessive distortion warnings.

 

[FEA way]

Try using tie constraint (available from the Create constraint dialog in the Interaction module). You just may have to disable adjustment and refine the mesh a bit.

 

[BrendaGR99]

I added contact control and that seems to keep the top surface in place. However, the results were excessive with the von mises results being up to e+4, I showed my boss at my internship and he said that I should change the body heat flux to a surface heat flux for more accuracy and he also made me change the boundary conditions to:
1. Displacement/Rotation BC at the bottom layer with U3=0
2. Displacement/Rotation BC at a point with U2=0
3. Displacement/Rotation BC at a point with U1=0

I ran the job and currently I'm receiving extreme distortion warnings and also the bottom surface is moving. I will upload the updated model.