Question about how contacts work together

[mcook21VD9DL]

Hi,

So I was wondering how can I mix auto/solver contacts with manually defined contacts? It's my current understanding that manual contacts take priority of those that are auto generated through the solver or automatic function.

My questions:

1. How do you avoid doubling up on contacts? How does inventor know not to create a contact that may make your manual contact irrelevant and therefore produce a poor result?

2. If I specify an edge to surface manual offset bonded contact (so that it knows that only the outside edges of the face are welded and not the entirety of the surface .. at least in my understanding) , will inventor NOT go and offset bond the entirety of the faces together, surface to surface?

Cheers

[mcook21VD9DL]

Anyone?

[John_Holtz]

Hi @mcook21VD9DL 

The number of possible arrangements and input is vast. I suggest that you do some testing on your arrangement to confirm that it is behaving as you want it to. (The contact force should indicate where nodes are connected. Although this does not indicate what the node is connected to, you will at least know if nodes that should not be connected have a contact force.)

Just to clarify for everyone's benefit, there are three commands in the ribbon for contact: Auto, Manual, and Solver.

•  "Manual" contact requires the user to select the geometry that is in contact, and define which is the master and which is the slave.
• "Auto" creates a manual contact based on which faces of the CAD parts are touching. Auto does not creating anything different than what the "Manual" contact produces.
• "Solver" will search the entire model (or only selected geometry) and create contact.

Now to your questions.

My understanding is that the nodes (and maybe the elements) that have contact elements created by manual contact are not available for use by the solver contact. So the edge-to-surface contact identifies the nodes along the edge, and these nodes cannot be used in the solver contact. (Perhaps the entire element connected to the edge cannot be used in the solver contact. A test model would need to be created to confirm that.) Naturally, this does not prevent the other elements on the face from being connected to the other surface. The best way to prevent excessive contact is to limit the maximum activation distance. See Understanding maximum activation distance and contact type in a Simulation.

• Edge 2 and Surface 1 are in contact using manual contact. Only node A will be connected to face 1.
• If solver contact is defined (either specifying surfaces 1 and 3, or not specifying any regions), then node A will not be connected to surface 1 by the solver contact. I do not know about node B which is on the same element as A. Nodes C and so on can be connected to surface 1 if they are within the maximum activation distance.

[mcook21VD9DL]

Hi John,

Thanks for your input. Would you perhaps recommend using a very low activation distance then for using solver contacts? Also, Let's say I choose surface to surface, and one of the surfaces (slave) I've chosen has a small (few mm) section of it that is not in contact with the master surface...might this be responsible for causing some inexplicable warp to my model? I've been using an activation distance of 6mm which may be excessive. Would this distance be trying to contact (up to 6mm) of the section that is technically not in contact (touching) the master surface and causing it to warp/wrap around the surface?

[mcook21VD9DL]

Hello again John,

I've just seen this article: https://knowledge.autodesk.com/support/nastran/learn-explore/caas/sfdcarticles/sfdcarticles/Understa...

With a mesh size of 4 and a face gap of 2, using pythagoras you need an activation distance of 5 to reach nodes. But what if your mesh is large like mine due to the object in question being large? I have a 30mm mesh and gaps spanning roughly 6mm. This means I'd need an activation gap of 31mm? But is this not too large of a gap?

[John_Holtz]

Solver contact does not use Pythagoras. The maximum activation distance needs to be larger than the gap between the parts (and probably larger than 0 for cases where the parts are in contact). Therefore, the max act distance is independent of the mesh size when using solver contact.

The manual contact needs Pythagoras. That does not cause a problem because you are specifying what geometry should be in contact. It will not generate extra contact between unintentional geometry like the solver contact could if you made the max act dist too large.