Showing results for 
Search instead for 
Do you mean 

Contact Parameters

[ Edited ]

I have a simple 3 point bend problem, but using SESTATIC-101 with Surface-to-Surface contact and friction of 0.2.

I am getting some unexpected results. I have kept most of these parameters default. Is this the problem?

I have attached a *.doc with these results. What contact parameters (or other solver parameters/conditions) should I use to prevent penetration or odd translations as shown?

Thanks in advance!

Jeff Morris
Manager, CAD/CAM/CAE

Re: Contact Parameters

Dear Jeff,
I understand you use NX Advanced Simulation, here you are my suggestions:
1.- The first thing to do is to study the problem using 1/4 model due to symmetry in loads & constraints. Split your model using symmetry planes, and prescribe properly symmetry constraint, this will increase the accuracy of the solution.

2.- Of course, mesh with hexaedral elements (CHEXA of 20-nodes), you will get much better results, more acurate due to mesh quality, tetraheral elements are a total disaster in contact problems. In this simply case not excuses to use HEX meshing, the geometry is simply.

3.- Define correctly the SOURCE/TARGET region: this is critical in contact problems, in your case the round part should be source, and the horizontal component should be TARGET.

4.- Mesh density: use the same mesh density in both SOURCE/TARGET regions, this is the best approach. Of course, specially in SOURCE region the mesh density should be refined.

5.- Please note you have a CURVED part contacting with a planar face: this is not trivil, but complex, the contact is a LINE, then to capture correctly the contact your model should be defined correctly. You must avoid undesired PENETRATION between SOURCE & TARGET, then set INIPENE = 3

If you want to learn more, take a look to my blog, all is there!!:

Best regards,

Re: Contact Parameters


Certainly great information and thank you for response. I would visit your blog - is there any chance there is an English version?

Thank You again.


Re: Contact Parameters


I would disagree with/adjust most of the points suggested in the original response.

1) Symmetry. I do agree with this. Modeling with 1/4 symmetry will stabilize the problem in the X and Y directions

2) While high order hex elements will probably produce a quality stress field with larger element size, I would not rashly dismiss using tetrahedron elements with contacts as a "total disaster". Parabolic tets are used successfully with correct results every day as long as an appropriate mesh size is used. Your overall mesh density looks appropriate for the problem.

- If you are interested in detailed contact pressures, you would want to refine the mesh in the area of the contact with either element type. This curved/flat interface degenerates into a line (Hertzian) contact problem which is a numerical singularity that produces rapid stress gradients.

3) Traditionally, source and target selection was critical and the best results were obtained when the mesh was matched on the two regions. Our NX Nastran refinement algorithm has all but eliminated this requirement. Assuming everything else remains linear (small displacement, small strain, finite sliding, etc.), the choice of source vs. target should not make that much of a difference. The refinement algorithm is producing a matched surface mesh internally in the solver.

4) This is good advice, but again, mesh density needs to be set more to pick up the stress gradient appropriately than to merely match mesh size between the two regions.

5) INIPENE=3 is entirely inappropriate for this geometry. This resets all initial gap and penetration values to 0 and effectively makes the cylindrical surfaces on the top of the supports flat planes. INIPENE=3 is only appropriate when the source and target regions are defined by coincident or translationally offset surfaces. Any difference in surface curvature will produce incorrect results.

Jim Bernard
Advanced Applications Engineer

Siemens PLM Software
2000 Eastman Dr., Milford, OH 45150-2712

Re: Contact Parameters

Dear Jim,
Total agreement with you, always learning a lot from you, not discussion from my end, perhaps the word "disaster" for TET elements is very radical, this is the result from experience dealing with contact problem, using HEX mesh allows to get quality results at a fraction of model size compared with TET models, and size counts when dealing with contact problems!!...
Best regards,

Re: Contact Parameters

Jim & Blas -

Thank you both for your responses. For me, the "why" is more important at this stage then just merely saying "use Tets" or "choose INIPENE=1" (or 3). The tutorials/documentation is not quite there with some of these clearer explanations that I receive from folks like you both.

1) If the Deformation scale is increased in the results plot, penetration is evident. Is this merely a cosmetic effect?

2) If the displacement is larger (let's say the force was increased) - would you recommend staying with the same parameters to maintain a "good" solution - or moving into another solution type or other parameter settings?

Re: Contact Parameters

Dear Jeff,
1.- This is a question of scale of deformations, plot deformed shape at scale 1:1 and you will see if penetration exist or not.
2.- The linear "surface-to-surface" contact on SOL101 is valid for small displacements only, if you increase loadings you will get a result of displacements & stresses, yes, but if displacement values are important then better run a nonlinear analysis (Advanced NonLinear SOL601 is the only that support "surface-to-surface contact) activating large displacement effect, this way comparing with the linear static SOL101 results will give you advice the accuracy of the linear static solution. Comparing different solutions is the best way to validate results.

Best regards,