Contact tolerance and showing automatic contact pairs

[Anonymous]

Hi. I have two questions:

1. where can I define the contact tolerance for the global contact settings (that affect faces which have a certain small distance but should have a contact)

2. is there an option to automatically generate and group contact pairs like in Inventor FEA?

Thanks

Marco

[AstroJohnPE]

Hi Marco,

For 1, look under "Mesh > Mesh > 3D Mesh Settngs > Options > Mode > Mesh Matchingl". When making a change, it is easier for me to set the "On-surface tolerance based on" to "Absolute length dimension" (that is, a dimension) and enter a value larger than the gap or overlap that exists.

But be careful that the value you enter is not larger than the smallest thickness in the model. Otherwise, you can collapse two faces to 0 thickness.

For 2, I do not recall exactly how Inventor does it, but there are two options in Simulation Mechanical.

a) Select two or more parts, right-click, "Contact > Create Contact Between Parts".

b) There is an option to detect and create ALL contact pairs when importing the model. Because of the length of time it takes to do this on a large model, it is off by default. But if you want it for some reason, look under "Tools > Application Options > CAD Import > Global CAD Import Options > Automatically generate contact pairs".

[tfjield]

Hi John,

I have a similar question...  I have a gap in my model that is 0.001mm.  I do not want the two parts to touch each other.  But even if I set the Mesh Matching to an absolute dimension and enter 1e-6mm, it STILL makes the two parts contact each other.

Any idea what I'm missing?

Thanks,

Todd

[Sualp.Ozel]

Try setting the contact type between the 2 contact pairs as "Free" or "Surface contact" prior to meshing the model.

[AstroJohnPE]

That's a bit strange Todd. It sounds like there may be an allowable lower limit that overwrites your input of 1E-6 mm.

Regardless of whether the mesh "matches" or not, Sualp's suggestion is always a good idea. That is, tell the software that the two surfaces do not contact each other (Contact type = Free). Even if the meshes match up somewhere, the solver will not merge the two nodes together.

A good example would be two cubes (same size) sitting on each other. The mesh has to match at the 4 corners. So if the software overrides the user and eliminates a tiny gap, the solution is for the user to tell the software that the two surfaces are really free.

FYI for everyone. Contact in general is described in the Help starting on "Mesh Models > Mesh Overview > Contact Pairs".

[tfjield]

Thanks, Sualp and John, for the suggestions.  I didn't understand how to use the contact pairing, so I ended up making the gap in my model larger.  Then I found that by using a percentage of surface mesh size, instead of an absolute size, I could make it not merge the two surfaces.

Based on the behavior, it wouldn't surprise me if there's a minimum value for absolute size that I wasn't aware of.

Do you happen to know, if I set the contact type as free and I'm doing a transient mass transfer analysis, will that prevent mass transfer even if the surfaces are in intimate contact?

Thanks again!!!

[Anonymous · Accepted solution]

Hey Jon,

great help. Thanks!!

Marco