Tool penetrating inner elements of workpiece

[Vxxxxx]

Hi! I am conducting 3D cutting simulation but my tool is penetrating inner elements of the workpiece.

Here are some settings that I used:
Step: Dynamic, temp-disp, explicit
Contact: general contact

I used to have this problem in 2D simulation but this forum helped solving that problem by using this code.

*Surface, type=element, name=xxx
,
yyy, interior
...
*Contact inclusions
xxx,
*Contact controls assignment, nodal erosion=yes

But for 3D model, I couldnt do the same as I could not select surfaces of inner elements.
It would be great if anyone could provide some guidance.
Thank you very much.

 

[Mustaine3]

It works the same way. You don't have to provide a surface, just an element set (=yyy).

Look into the documentation:
Abaqus > Abaqus Introduction & Spatial Modeling > Spatial Modeling > Surface definition > Element-based surface definition

 

[Vxxxxx]

Hi Mustaine3, thank you very much for your reply.

I tried the same thing, which is:

*SURFACE, NAME=surface_name, TYPE=ELEMENT
element_set_name, INTERIOR

*Contact inclusions
surface_name,
*Contact controls assignment, nodal erosion=yes

but it still doesnt work.
Abaqus Error: Analysis Input File Processor exited with an error.

Thank you.

 

[FEA way]

Check the msg, dat and sta files. They usually contain more specific errors that can give you a hint about what’s going on.

 

[Mustaine3]

Works fine in my test. I've used this for the general contact definition:

*Contact, op=NEW
*Contact Inclusions
,
,surface_name

 

[Vxxxxx]

Hi, after several testing, it worked. Thank you very much, Mustaine3 and FEA way.