How to connect different meshes with INTER/TYPE2

EG_21092

Hello,

Here is my issue: I want to change the mesh of a given part of interest in my model (green). I re-meshed it and now I would like to manage the interaction between my new mesh and the coarse mesh (grey) of the parts in contact with it (cf. screenshot).

I have been advised to use an INTER/TYPE2 interface. I tried to implement it but I didn’t succeed.

Should I take my part of interest (green) as master surface (Surf_id)? The tool proposes to select it by elements/set/component. The “by elements” option only works with shell elements, that I don’t have originally in my model.

For the Grnod_id (S), the selection by nodes works.

Also, which parameters would you recommend for this INTER/TYPE2? (Are the 0: default values ok for this kind of application?)

 

Thank you for your help.

PaulAltair

I assume from your comments that you are showing solid meshes? The easiest way to do it would be to select your green part 'by component' then select only the nodes of the secondary grey part as secondary

Recommendations for the other options below:

set ignore = 1 (so any nodes that cannot find a projection are ignored without an error being generated)

Set spotflag = 27 (this uses 'kinematic conditions' if possible but will use penalty method in case of any conflict with another kinematic condition on the nodes/elements of the contact (e.g. another tied contact, RBODY or BCS) this again minimises chance of your contact creating an (incompatible kinematic condition) error.

It looks like your meshes are very close (co planar?) so you should set dsearch to a small value, e.g. 0.1mm, so that nodes aren't mistakenly tied if they are further away (no nodes further from this distance normal to the main elements will be tied

If you have any element failure defined, you can set idel2 = 2