Non-Linear Static Analysis Convergence Issues

[jstillingULA5U]

Hi All,

I'm trying to run a simple gasket compression analysis, and I can't seem to get "load convergence" for the first increment causing a "Maximum Number of Bisections reached" error.  I'm new to Nastran, so I'm probably missing something pretty fundamental with the setup.  Can someone please take a look at the attached file?

Simulation Properties:

Applying an Enforced Motion on the aluminum block of -.25" in the Y-direction

Using Hyperelastic material properties for the Silicone Rubber Gasket

Allowing translation in the X and Z directions for the gasket bulbs but constraining all other DOF

Allowing translation in the Z-direction for all faces of the aluminum block except the enforced motion face (this is fully constrained)

Bonded contacts for the aluminum-gasket surfaces in contact and separation contacts for the portion of the gasket bulbs that will come into contact with the aluminum

[John_Holtz]

Hi @jstillingULA5U 

The .iam is not the complete model, so no one can see the model. You need to include all the part files (and any subassemblies) that are referenced by the assembly. The safest method is to use the steps in What files to provide when the model is needed - Autodesk Community. (For a simple model where all the files are in one folder, simply attaching the part files, or compressing the assembly and part files, can also be done.)

John

[jstillingULA5U]

John,

Thanks for reaching out.  I've attached all of the files required for the assembly.

Regards,

Jack

[John_Holtz]

Hi Jack,

Where did you get the material properties? The default value for D1 is 1000*(A01+A10). Your value is 0.0083 times (A01+A10) and seems wrong. (D1 is similar to the bulk modulus for a material; it controls the volumetric compression of a material which is usually 0 for a rubber material = infinite bulk modulus.)

Also, I was having problems with the manual separation contact between the steel and rubber. Something was blocking that contact from getting to the Nastran file. I had to delete the Manual Contact [4] and re-create it. If you get a warning related to this contact when you try to run the analysis, you should do the same thing. (If you are not getting a warning, it must just be my computer.)

The next issue may be getting the analysis to converge. The material may be trying to buckle, or the compression strain may be trying to collapse an element.  We will deal with that if it occurs.

John

[jstillingULA5U]

Hi John,

Thanks for the insight, for the material properties, it appears AI has failed me.  I was unsure what to put in those boxes and it looks like I was steered in the wrong direction.

I re-ran the simulation using default values for A01, A10, and D1 and it still failed to converge on the first increment.  I've attached a screenshot of the error messages.  Please advise!

[John_Holtz]

Hi Jack.

What do you mean by "default values for A01 and A10"? Those two values do not have a default. (Okay, maybe Nastran defaults to 0.0, but that is meaningless.)

If you do not have real material properties, you are wasting your time trying to use a hyperelastic material properties. Another customer said the following in regards to determining the hyperelastic coefficients:

• Data from many suppliers is unreliable.
• When labs provide testing for FEA, they have to tweak the constants so that they work. (To me, this implies that even with sufficient lab test results for tensile, compression, shear tests, and so on, you may still need to adjust the constants.)
• Try the following "balanced" Mooney Rivlin constants. A01=0.15; A10=0.6; D1=25. If the model runs with these constants, then the loads, constraints, and mesh are probably okay. If the analysis fails, the mesh, contact, etc is causing a problem, and the analysis will not run with real material properties. 

But of course, you do not want to use the "balanced" Mooney Rivlin constants for the final analysis because who knows how closely those constants apply to your material. If you have the stress-strain data suggested in this article, you can input the stress-strain data. See How to enter hyperelastic (rubber) materials in Nastran. If you do not have the required stress-strain data, you should just use an isotropic material with a Poissons ratio set to 0.48. (Real rubber has a Poissons ratio of 0.5, but that value does not work in a simulation.)

I tried with isotropic properties (E=435 psi from material library, Poissons = 0.48) and a coarse linear element mesh. The analysis got to 47% complete before it failed. It may require a much finer mesh, or the amount of compressive strain may be too large for the analysis to handle. I suggest making the model 1/10 the length so that it runs faster. There is also half symmetry about the YZ plane, so cutting it in half would also reduce the model size. (Once you get the small model to run, you can run the full model overnight if you want to show that result to a customer, for example.) If using a parabolic mesh, you will want at least 2 elements through the thickness of the door seal for the final run. If using a linear mesh, you want 4 or more elements through the thickness. (I do not know for sure, but I'm guessing that linear elements are less prone to buckling than parabolic elements.)

John

[John_Holtz · Accepted solution]

I sliced your model. The nonlinear static analysis got to 63% complete before failing. Time to try something different.

The solution is to use an Explicit Dynamics analysis type (or Explicit Quasi-Static). See the last analysis in the attached model. It solves in about 5 minutes.

• The nice thing about the Explicit Dynamics is that it does not require convergence. It has a much better chance of success. (The "only" reason it would not succeed is if an element distorts too much, or a program bug.)
• The downside is that it requires a really small duration, so the dynamic effects can be a problem in some cases. (My duration was 0.001 seconds, which may not be too bad if this is a door slamming shut.)
• The advantage of a really small duration is you can make the event as short or as long as you want, and the run time is proportional. Use a short duration (like I did) to see what happens. (The bonding between the steel and rubber looks odd, unless the two are physically glued together.) Once you have one analysis, you will know how long you can make the duration to get a runtime completed within X minutes or hours, if desired.
• Once you have a working model, you can also change to Explicit Quasi-Static if you want the solver to calculate "what duration is a fair approximation of a static condition". Note that quasi-static runs the analysis 2 or 3 times (with a longer duration each time), so the runtime can be much longer than a "quick explicit dynamics" analysis.

Note: I use a rigid body connector in some of my analyses. For unknown reasons, the rigid connector was not working in the explicit analysis. I applied the enforced motion directly to the face (just like in your original setup).

John

[jstillingULA5U]

Hi John,

Thank you so much for sharing your expertise, this will certainly suffice for now.  I appreciate it!

Regards,

Jack