Learning Forum

[michealpin]

I am designing an assembly that has a rubber part which is manufactured in a 'flat" shape, then stretched over another spring-like part forming an assembly.  When initially assembled, the stretched part imposes a compressive force on the spring part, counteracting the spring and compressing it slightly.  This is a system of two opposing forces.  I can simulate the stretched part and the spring part separately but would now like to try and build the assembly of both parts in one model.

[Akshay Maniyar]

Hi Michael,

Thank you for posting. Can you share some inline images for a better understanding of the issue? 

Meanwhile, you can check below KM for including initial stresses in the model.

How to apply initials stress on a deformed geometry in Workbench Mechanical? - Ansys Knowledge

Thanks,

Akshay maniyar

[michealpin]

Akshay - thanks for answering.  I've included a simplified representation of the problem.  Meanwhile I'll check the KB link.  Thanks!

[michealpin]

I opened the Workbench model provided in the KB link and understand the example.  The two models (static structural and transient structural) both use the same model (one is pre-stressed, the other uses that as an inuput). 

Is it possible for the originating (pre-stressed) model to feed into a more complex model that includes the pre-stressed part as one of the components?  That is my situation.  Please see attached.  Thanks -

[peteroznewman]

Michael,

The following workflow assumes Part #1 and Part #2 analyses are in the same Project Schematic and each one is meshed. The benefit of this workflow is reusing the time invested in meshing the two parts.

Drag a Mechanical Model from the Component Systems part of the Toolbox.  Drag the Model cell from Part #1 onto the Model cell of Mechanical Model to create a link.  Repeat for Part #2.  Then drag and drop a Static Structural analysis onto the Model cell of the Mechanical Model.

If the geometry for Part 1 and Part 2 was created so that Part 1 sits on top of Part 2 before any deformation has occured, then you don't need to edit the Mechanical Model.  If that is not the case, you can right click on one of the parts and Insert a Part Transform and move the parts into that configuration.

In the new Static Structural, you can apply a support to Part 2, and a Displacement to the edges of Part 1 to move that down into a state of interference.  Add a Frictional Contact between the top and two blends on Part 2 as the Contact side and the flat face of Part 1 as the Target side of the contact pair.

If remeshing the two parts is a trivial amount of time, just put both parts into the same geometry file (SpaceClaim) then build the model described above in a single Static Structural model.

[michealpin]

Peter,

Actually your idea completely solved my issue (which had to do with my "frame of reference" in the assembly as you suggested).

I'm going to approach this from a different angle. 

Thank you.