Difference between surface contact mesh and mesh mating condition 2

[prakhar5aug]

Hi,
what is the difference between surface contact mesh and mesh mating condition and when are they applied.....
I have two welded sheets which must not pass through each other...

 

[BlasMolero]

Hello!,
Well, this is a question related with meshing on NX Advanced Simulation, not directly with NX NASTRAN solver, but I will try to explain (by the way, all is in the manuals ..):

• MESH MATING CONDITION: this is a task done in the FEM environment of NX AdvSim, at the meshing level, simply performing maesh mating condition command between two parts of an assembly will create imprints in the geometry to make sure that both meshes are coincident (matching) and then node merging will be performed at the meshing time to satisface the continuity on displacements condition between both parts. if for any reason the mesh could not be coincident, then multipoint constraints or rigid elements will created by the mesher to allow gluing both parts. But remember, all is done at the meshing level (FEM environment). You have three options:
- Glue Coincident condition: makes both the geometry and the meshes match between the source and the target faces.
- Glue Non-Coincident condition: the mesher creates connections between the meshes on the source and target faces.
- Free Coincident condition: the mesher aligns the meshes on the source and the target faces. The software does not create any connections between the meshes.

• SURFACE-TO-SURFACE CONTACT: this task is donde in the SIM environment of NX AdvSim, here you can define a GLUE surface-to-surface contact between SOURCE and TARGET regions, or NO PENETRATION surface-to-surface contact between regions. The GLUE condition allows to define a rigid joint between two surfaces, where the NO PENETRATION CONTACT condition prevents the penetration between regions but allows to freely separate. This task is done during the solution phase of the NX NASTRAN solver.

You can either specify the contacting surfaces manually, or you can have the software automatically determine which pairs of faces come in contact with each other.
- To manually specify source and target surfaces in the contact definition, you can select an existing Simulation Region or create a new one.
- To have the software automatically determine the contacting surfaces, you can use the Create Automatic Face Pairs dialog box to specify the criteria the software uses to search for surfaces.

Best regards,
Blas.





~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[prakhar5aug]

Hi,
thanks for the detailed reply but I was asking about the surface contact mesh in FEM environment not the surface to surface contact in SIM environment of NX ADV simulation.

Prakhar Gupta

 

[BlasMolero]

Dear Prakhar,
SURFACE CONTACT MESH is an older method of creating contact 2-node CGAP elements, is an old fashion method (that I continue using, specially with FEMAP !!) but is tricky, requires that nodes from both parts to be properly aligned, is not easy, only runs with mapped mesh, forget to use this method with automatic meshing, this is only for experts. Also you need to define correctly the orientation vector and properties of the CGAP element.

Surface-to-Surface Contact compared to Surface Contact Mesh??
As explained, when the solution is set to the NX Nastran solution type SOL 101, there are two commands for defining surface contact:
•Surface-to-Surface Contact, when a Simulation file is active.
•Surface Contact Mesh, a legacy command, when a FEM file is active.

You should use always Surface-to-Surface Contact to define contact between two surfaces, not any additional meshing action is required, all is done by the NX NASTRAN solver at the execution level. Unlike Surface-to-Surface Contact, Surface Contact Mesh generates contact 2-node CGAP elements between the two surfaces.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[prakhar5aug]

Hi,
I have got your point but with surface to surface contact in sim environment the solver run for about 7 hrs and gave no result, I have also tried automatic surface contact mesh in fem environment with iterative solver though it didn't converge but gave fairly good result.

I am using NX 7.5, my doubt is applying these contact mesh will it affect the weld mesh which are there in the contact region and if yes what will be the effect.

Is there some command or constrain that tell nastran that this is a sheet do not pass through it......

Thanks & Regards
Prakhar

 

[Tuw]

Hi Prakhar,

If you are running sol101, and the contact is closely in touch (meaning no shrink fit or physical gap in between), and you wish to get a quicker result, I would suggest you change all your contact definition into glue definition.