I have been working with linear contact problems for a while now. When the contact is between two parallel surfaces it works well. But when I have 3D surfaces in contact the peak stresses are unreasonably high. When refining the mesh the stresses get lower but to get a sufficient result the mesh size would be 0mm. My thought is because the 10-node tetrahedral elements will act like a linear interpolation of the surface.
Do any of u guys have any good tips for me to get ridd of these unreasonable peak stresses?
Would it help changing the Min Contact Search Dist from 0 to 1e-5?
Solved! Go to Solution.
In linear contact the INIPENE parameter is critical, take a look to my blog in the following address: https://iberisa.wordpress.com/2012/01/14/mejora-de-resultados-de-contacto-lineal-con-inipene-en-fema...
Also, to reduce the model size use when available HEX-8 elements instead TET-10 elements, this is my best recommendation. To avoid unwanted mesh interferences you can deal with INIPENE parameter, but the best method is to get matching mesh between contacting bodies, this way the unwanted & artificial mesh interference will disappear. As you say, in planar contact the effect disaapear, but in curved surfaces the interference problem exist, and is the reason of most of the problems of hot-spot stress.
Of course, when using high-oder mesh elements like CTETRA 10-nodes or CHEXA 20-nodes make sure that midside nodes are located in the geometry, in the exterior surface of the solid, OK?.
Also the following post will let you know how to deal with INTERFERENCE-FIT problems using FEMAP & NX NASTRAN solved with Linear Static Analysis (SOL101):
Thanks for the help Blas!
Changed INIPENE to 3 and the high peak stresses disappeared.
Really appreciate all the great work you do for the Femap community Blas.