Learning Forum

[aminuddin setyo]

hi..

im doing grid independent test in my hip implant analysis

why does the von misses stress result always increase when I reduce the size of the mess? even though in the reference journal that I use, there is no significant change in the von misses when reducing the size of the mess
Here I include the settings that I use, maybe someone here can help me...

[aminuddin setyo]

[aminuddin setyo]

[aminuddin setyo]

[aminuddin setyo]

[peteroznewman]

It would be more helpful if you show the mesh where the peak stress is found and explain any boundary conditions, loads or contact elements near that region.

[aminuddin setyo]

the boundary is have force in top of hip imlant with 2300 N resultant force, and the botom part (bellow 80+10 mm) is fixed suport

(stem is cut into 3 parts like this)

[aminuddin setyo]

 

A resultant force  of 2300 N (1800 N in Y direction and −1420 N in X direction) was applied on the surface of the 
backing cup and the bottom part of the stem was kept fixed in all degrees of freedom

 

A resultant force of 2300 N (1800 N in X direction and −1420 N in Y direction) was applied on the surface of the backing cup and the bottom part of the stem was kept fixed in all degrees of freedom

 

[aminuddin setyo]

the mesh where the peak stress is found is like this

when the mesh size is reduce, the stress is keep increase

 

[peteroznewman]

You have a stress singularity. That means that the theoretical stress is infinity, so each time you reduce the element size, the stress increases.

To remove the stress singularity in the implant, don't use bonded contact to hold the three pieces together. Open the geometry in SpaceClaim and use the Share button on the Workbench tab to create Shared Topology and delete all the contacts from the model.

To remove the stress singluarity on the implant, don't use Fixed Support on the bottom half of the implant. In SpaceClaim, add a cylinder that represents the bone up to the height of the lower portion of the implant. Subtract the lower portion of the implant from the cylinder. Use the Share button to connect the implant to the bone part. Use a Fixed Support on the bottom circular face of the bone.  Assign bone material properties to the cylinder.  When you plot the stress in the implant, don't include the bone part.

[aminuddin setyo]

thank you s much sir

 

[aminuddin setyo]

but sir, how about my frictional contact in femoral head and stem?? Will the contacts also be deleted?

[peteroznewman]

No, keep those.

[aminuddin setyo]

sorry sir, can this stress singularity be avoided simply by adding a Shared Topology and deleting all the contacts from the model without providing additional cylinders as bones for fix support?
because the reference journal that I use does not use the additional bone cylinder
like this

[peteroznewman]

You can try it and see. The problem is a fixed support is infinitely stiff. That is why I suggested a layer of bone to isolate the implant from the fixed support.

Maybe what the journal does is only report the stress in the green and gray parts, and excludes the stress in the brown and blue parts. If you do that there is no singularity in the reported stress. It is in the brown part which you are ignoring. That is another way to do it.

[aminuddin setyo]

ok sir..

 

[aminuddin setyo]

actually in journal report, it use total von misses stress on hip implant for grid independent study