Problem in boundary condition to move object as the result of external pressure

[SM1994]

Hello
I am trying to simulate a force being applied on a cylinder inside an object encompassed by another semi-conical shape object.
Sorry, to make the explanation clearer, I named the parts (objects) inside the model and attached its image.
Similar to the attached image:
Object A is tied inside object B. There is a 2mm clearance between object B and object C, and the interaction between object B and C is surface to surface contact with the friction of 0.5 and normal hard contact.
There's no boundary condition on object B, but the outer side of object C has an encsatre (no move at all) boundary condition.
I apply pressure on the top of object A, and it squeezes object B internally, but I expect that as a result of this external pressure, object A and B moves down until object B and object C come into contact, but it does not happen and the object B does not move.
Does anyone have any idea why it happens, and what should be the boundary condition that object B moves down toward object C as the result of pressure being applied on object A?
Thanks

 

[FEA way]

Try with lower friction coefficient and displacement control instead of load control first. Maybe the movement is too small to be noticed - check the deformation scale factor and contact outputs (CSTATUS, CPRESS).

Is this gap between B and C absolutely necessary ? It may cause problems.

 

[SM1994]

Thanks for your response.
I have checked with displacement control, but there was no difference. Since the change in the stress on contact between objects B and C is absolute zero.
there should be an initial clearance, then after applying the force and the object B comes down, B and C should come into contact.

 

[FEA way]

Can you share the .cae or .inp file ? If not, screenshots of the results (with scaled deformation) can be useful.

Is that a simulation of some real-life assembly process ? Something related to prostheses ? What are the material models ?

 

[SM1994]

Hi
I have attached the CAE file.
You can download the ODB results from here.
Yes, it can be said that object A is a bone, object B is a residual limb and object C is a socket for that.
Object A has steel properties.
Objects B and C have hyperelastic properties.

 

[FEA way]

I checked your model. Here are a few remarks:
- make sure that all units are consistent. For example, if you use the SI(mm) system, the density should be in tonne/mm^3. It seems to be incorrect in your case.
- you could use symmetry and solve just a quarter of this model
- mesh all parts with hexahedrons (some parts will require basic partitioning with datum planes first)
- there is a large intersection between the bone and the stump. Is it necessary ? It can cause problems.
- I would replace the contact pairs with general contact
- the gap between the stump and socket may be problematic even for a dynamic implicit step. Check the warning messages and make sure that Abaqus can handle the model correctly.
- consider rounding the bottom edge of the stump - sharp edges can make it stuck in contact with the socket causing further convergence issues

 

[SM1994]

Thank you for your help.
You are right, the density unit was wrong. I changed it and it is working ok.