Learning Forum

[RoyalFlowers]

Hello eveyone,

I have a question regarding stress distribution contour and would be grateful if somone could help me about that.

When we would like to interpret von-Misess stress contours, first of we payy attention to max values. But sometime like the bellow picture, the masx stress is samll red spot. Even the mesh size is small enough, still there is this single point. Hence should we report the value of this small area as max. stress value or should we go 3 to 4 nods furthur and then report stress values in th area with more uniform distribution?

Also, if we want to report the mean Von-Mises Stress for the plate for example, how could we do that?

I would be thanksful if somone could advise me in this regard.

Sincerely, Shabnam Samsami 

[peteroznewman]

What is the load that is causing the hot spot?  Does it accurately represent how the material sees the load such as frictional contact with another body not shown, or is it a simplified boundary condition that is a crude approximation of how the material sees load such as a Fixed Support?  In the former case, then the hot spot is real and there is no merit in moving away and ignoring it.  In the later case, if the stress is a concern, build another model to represent that interface more accurately.

What is the material and how does it fail?  If it is a ductile material, it has a yield strength, so the maximum von Mises stress can show if the material has yielded. The "hot spot" is where yielding will begin. In fact, if you do a Mesh Refinement study, the peak stress may increase as the elements get smaller. If it is a brittle material that suddenly fractures, maximum Principal stress is more relevant than von Mises stress.

What material model is used in the simulation? Is it Linear Elastic properties only?  If a ductile material has gone past yield, you can add Plasticity to the material model and the high stress will be gone, replaced by plastic strain.

I don't use mean stress. When I have seen it used, it is computed on a cross-section construction plane.

[RoyalFlowers]

Dear Peter,

Thanks a million for your illumination answers.

-The following picture shows loading and boundary conditions

The plate in which stress distribution was evaluated was attached with some screws to bone. Screws have MPC contact with plate holes, and there is no contact between plate and bone surface.

The applied load results in screw bending and because bonded contact between diagonal screw and plate hole (highlited in below picture) act as a fixed support, there is a stress concentration around plate hole as it is shown. And Max von-Misess stress happended arround this hole. 

-As you said, this stress concentration occured due to boundary condition and I think that I can report this max stress value and I should not go furthur a way to report stress. Is my interpration correct?

-Loading is linear and all materials are assumed as linear elastic.The plate material is Titanium alloy and it is ductile material, hence we want to evaluate von-Misess stress distribution to compare the effect of bone fracture geometry on the load transfer and stress ditributions of the plate. Of course the fracture geometry has an effect on Von-Misess stress distribution of plate. If Max. stress value is closer to yiels strength of plate material, there is a sign of plate failue in that area. Are you agree with me?

-My another question in this regard is that since we do not do any plactic or material strength evaluation, Doess it make sence to report von-Misess stress counturs  or is it better to focous on von-Misess strain instead of that?

-What is your recommendation if we want to report stress of plate only as one value?

I am grateful for your kind attention regarding my questions in-advance. 

Sincerely, Shabnam

[peteroznewman]

What is the yield strength of the titanium alloy?

In the physical world, is the screw head actually bonded to the plate at location G? If not, Bonded Contact at point G results in a hot spot that does not accurately represent the stress around that hole. To get a more accurate representation of stress around that hole, you will need Frictional Contact. That change may cause convergence difficulty because you are changing from a linear contact to a nonlinear contact. But if the screw head is not bonded in the physical parts, then wouldn't the force at the top cause the screw head to open up a gap to the plate?

If the screw head is actually bonded to the plate, then the strength of the glue bond may be the weakest link, not the strength of the titanium. What is the strength of the glue?  How has that been determined?

In either case, you need to perform a Mesh Refinement Study to see how stress changes with element size.

If you have linear materials, look at von Mises Stress and compare with yield strength.  If you enable plasticity in the material model, then you look at Total Strain and compare that with elongation at break.

 

[RoyalFlowers]

Dear Peter,

Thanks a gain for your answer

Regarding contact between screw heads and plate holes, since in the reality there are threads around each screw head and plate hole, we assumed the bonded contact between with MPC formulation for screw head and plate hole. Because we didi not model screw and hole threads and modeled them as simple cylinders with MPC contacts.

Regarrding the element size, I check the max. von-Misess stress of plate and hole by increasing the element size of plate and refined element size of hole G but the Max stress values did not converged. Hence I think that this Max stress point is a singulaity. On the other hand, the average and unaverage von-Misess stress values are not the same, and it confirmed again that this Max. stress point is a singularity. Hence, stess evaluations should be perfomed some nodes a way from this singulaity in which average and unvarge von-Misess stress values are not significantly different. I am grateful in advance if you could help me in this regard.

Best regards, Shabnam

[peteroznewman]

Dear Shabnam,

Replace the bonded contact at G with a Fixed Joint.  Pick the hole first to put the joint coordinate system at the center of the hole. Pick the face of the screw head for the other side of the joint.

The benefit of a Joint over bonded contact is that you can easily request the total force going through the joint using a Joint Probe. In a hand calculation, evaluate the ability of the threads that have not been modeled to withstand stripping under the computed force.

Both Joint and MPC bonded contact are going to have a similar stress hot spot effect on the face of the hole. You can set the Joint behavior to Rigid or Deformable. Try it both ways. Since the threads are not modeled, it is reasonable to ignore hot spots around the hole.

Best regards,
Peter

[RoyalFlowers]

Dear Peter,

Thanks a million for your helpful answer.

I agree with you that the hot spots arround plate holes occured due to ignoring threads and simplifying that with MPC bonded, hence these singularites can be ignored.

Also, I would like to ask you that only for evaluation stress as an estimation about load transfering is it better to calculate voo-Mises Stress or Principla stress?

Best regards, Shabnam

[peteroznewman]

For a ductile material, von Mises is the best metric to use to compare with Yield Strength or Ultimate Tensile Strength.

[RoyalFlowers]

Dear Peter,

I really do appreciate your advices.

Best regards, Shabnam

[saifali]

Please share the file