Defining Explicit Surface to Surface Contact In an Import Analysis 1

[luc46552]

Hello, I've been trying to import the results from a standard analysis into a new explicit analysis for the final step. I was having trouble writing the input file for the explicit analysis, and I have narrowed the issue down to one problem. I have reviewed the Abaqus documentation and have posted here before, but now I have narrowed the problem down to a contact definition.

I have a simulation with two parts in contact. In a static, general step, one part is bent over the other part through a displacement as shown below. After that, the results are imported to an explicit model by running a job as an input file containing the *IMPORT command. In the explicit step, the displacement BC is removed and the bent parts are allowed to spring back to their original position.

The root of all these problems seems to be the contact definition that I am using between parts. This analysis is somewhat short, so I will post the entire input file (except the heading) since I'm not sure what is and isn't useful. When the job runs, it successfully imports all instances, defines all surfaces, and enforces the boundary conditions. However, it returns the errors

"An invalid surface name has been specified with *contact pair"

"A blank data line cannot be specified under *surface if it is used in *contact pair."

"Contact pair references surface/node-based surface/analytical rigid surface assembly_stick-back but this surface/node-based surface/analytical rigid surface cannot be used with *contact pair. Check previous warning messages for this surface to find the cause."

It almost seems like the job is not recognizing the assembly-side surfaces defined in the input file. However, the surface sets appear in the ODB, and when I import the ODB as a model the surfaces are clearly defined, which leads me to believe that the surfaces do exist in the explicit model. Any help is appreciated, thanks.

*ASSEMBLY, NAME=Assembly

*INSTANCE, INSTANCE=Stick-1, LIBRARY=StickTestImplicit
*IMPORT, UPDATE=NO
*END INSTANCE

*INSTANCE, INSTANCE=Stick-2, LIBRARY=StickTestImplicit
*IMPORT, UPDATE=NO
*END INSTANCE

*SURFACE, TYPE=ELEMENT, NAME=Stick-Front
Stick-1.Stick_Front
*SURFACE, TYPE=ELEMENT, NAME=Stick-Back
Stick-2.Stick_Back

*END ASSEMBLY


*Surface Interaction, name=Contact_1

*Friction
0.2,
*Surface Behavior, pressure-overclosure=HARD

*BOUNDARY
Stick-2.Stick_Right, ENCASTRE
*BOUNDARY
Stick-1.Stick_Right, ENCASTRE
*BOUNDARY
Stick-1.Stick_Left, ENCASTRE


*STEP, NAME=Release_Stick, NLGEOM=YES

*DYNAMIC, EXPLICIT
, 1
*BULK VISCOSITY
0.06, 1.2

*Contact Pair, interaction=Contact_1, mechanical constraint=KINEMATIC, cpset=Contact-1
Stick-Front, Stick-Back

*END STEP

 

[FEA way]

Standard and Explicit solver in Abaqus use different contact formulation and this may lead to errors. Can you try with general contact instead of contact pair ?

 

[luc46552]

That absolutely worked. Interestingly, the reason the surface contact wasn't working was actually a formatting issue. There can't be any empty space under the surfaces listed under *CONTACT PAIR, but general contact actually makes things easier for what I am trying to do.