Stress Singularities on curved parts

[Anonymous]

Hello,

I am currently trying to analyse results from simulations on a wheel. The problem is, I have stress-singluarities on curved parts , in the interface wheel-axis.I don't understand why ; I have tried to re-mesh the contact zone more precisely, but it only seems to change the location of the singularity.

I have seen that stress-singularities can be found on edges or nodes, in particular if there is a constraint or a load on them. Here the constraint is a contact surface between two parts so I don't know if it is the same problem . I don't think it is because the stress maximum seems ton converge, but its location  changes with the location of the singularity.. I changed the contact distance in advanced parameters to 0.0003, but otherwise I didn't change any contact parameters.

My question is :
- are those singularities logical? if not is there a way to eliminate them, by another mesh for instance? 

- is it possible to draw conclusions without running other simulations ?

    In that case, should I say : - those singularities should not be taken into account at all ?
                                             - those singularities may happen somewhere on the part, so I should take into accound the intensity of the stress but not                                                  its location ?

Of course in reality my part will never be a perfect cylinder so maybe the singularities would happen indeed.

I use Autodesk Simulation Mechanical 2016, and join some images of the model and results. I used symmetry in the XZ and YZ plan to symplify the model.

Thanks for any answers you could have 😃

Marie Malafosse

[AstroJohnPE · Accepted solution]

Hi Marie,

It looks like you are performing a nonlinear analysis (either MES or nonlinear static) and using surface-to-surface contact. Is there a gap between the axle (part 3 per the name of your image, but looks like part 5 based on the color I see in the model image) and the wheel part (part 1 per the name of your image, but looks like part 4 based on the color I see in the model image)? If there is a gap, I suggest that you eliminate it.

I agree with you that the stress concentration is not realistic. You could ignore it, except the concentration indicates that there is an extra force in the system, and that extra force may be affecting other results. (You can check the contact force using "Results Contours > Other Results > Element Force > Axial" to see the contact force.)

I think the concentration occurs because the meshes do not match on the two parts. (This is either a problem with the mesher, or because there is a gap between the parts that is "forcing" the mesh to not match.) If you hide all of the surfaces except for these two surfaces in contact, you might see that the mesh does not match at the location of the stress concentration.

If the meshes are not identical on the two curve surfaces, then you can get mathematical interference. (The attached image is from the page "Surface-to-Surface Contact > Advanced Controls" in the Help documentation. Although meant to show how the mesh can intefere when two cylinders are rotated, a similar problem can occur if the meshes do not match to begin with.) If there are a few points that do not match, you might be able to move the vertices manually ("Draw > Modify > Point Move") to avoid the interference.

[Anonymous]

that seems to be the problem indeed... I had chosen not to match the meshes because of the page Surface to surface contact > tips, in which it is said that it is not a good idea for MES simulations(https://knowledge.autodesk.com/support/simulation-mechanical/learn-explore/caas/CloudHelp/cloudhelp/... Could you explain to me in which case this advice is correct ?

However when I tred to refine the mesh on the new maximum-stress which is on an edge, the simulation goes wrong and I don't know what this new problem is about...

I attach the new appearance of the parts ( you are right I did not name the part correctly..), and the new problem when I re-mesh (I just added refinement points on the points where there is a maximum stress, passing from elements ~5mm to 3mm)

Thanks for your answer!

[AstroJohnPE]

Hi Marie,

The image "Simulation_remeshed.png" shows that some of the elements are hidden; that's why the parts look like a jumbled mesh. You need to show all of the elements, either by "Results Options > View > Element Visibility > Show All", or by right-clicking on the part > "Visibility" until the checkmark is solid. (No checkmark on "Visibility" indicates that all elements are hidden, a gray checkmark indicates that some elements are hidden, and a solid checkmark indicates that all elements are visible.)

[Anonymous]

That seemed to be it., thank you very much.

However I have realized that remeshing with matched mesh caused another problem for the surface contact with the ground.
when the meshes were not matched, I had an elliptical shape for the maximum stress on the ground. ( I think that's that's what the result is supposed to be) . However, now that the mesh are matched, the maximum stress are on a line relatively far away from the center, and near the edge, the stresses are quite low.

(to understand the images ; I reinforced the wheel by a thin layer of iron which is cylindrical and 5mm thick). 

To understand the difference in the stress repartition,  i zoomed on the mesh and there is a zone where the mesh of the reinforcement comes downward, at an lower level than it should be ( I try to show it on the image I join). This location is exactly above the maximum stress on the ground.
I tried to remesh the reinforcement on this line ,so that the geometric irregularity of the mesh would disappear, but it just displaced it.

Is there a way to specify that one surface contact zone should have matched mesh and not the other?

Or should I keep the values I had on the first simulation for the ground ? However there is a huge difference between the maximum stresses; when the meshes were unmatched, the maxium stress on the ground was about 20MPa and with the mesh matched it is now 7Mpa

[Anonymous]

That seemed to be it., thank you very much.

However I have realized that remeshing with matched mesh caused another problem for the surface contact with the ground.
When the meshes were not matched, I had an elliptical shape for the maximum stress on the ground. ( I think that's that's what the result is supposed to be) . However, now that the mesh are matched, the maximum stress are on a line relatively far away from the center, and near the edge, the stresses are quite low.

(to understand the images ; I reinforced the wheel by a thin layer of iron which is cylindrical and 5mm thick). 

To understand the difference in the stress repartition,  i zoomed on the mesh and there is a zone where the mesh of the reinforcement comes downward, at an lower level than it should be ( I try to show it on the image I join). This location is exactly above the maximum stress on the ground.
I tried to remesh the reinforcement on this line ,so that the geometric irregularity of the mesh would disappear, but it just displaced it.

Is there a way to specify that one surface contact zone should have matched mesh ( in the wheel axis) and not the other (wheel/ground interface)?

Or should I keep the values I had on the first simulation for the ground ? However there is a huge difference between the maximum stresses; when the meshes were unmatched, the maxium stress on the ground was about 20MPa and with the mesh matched it is now 7Mpa

[AstroJohnPE]

Hi Marie,

At one time, there was an option, something like "don't match the mesh when not necessary", or "match the mesh when appropriate". The software know that if the analysis was linear and surface contact was defined, the mesh needed to match, but if it were nonlinear and surface contact was defined, the mesh did not need to match. So,

• look to see if something like that exists under the "Mesh > Mesh > 3D Mesh Settings > Model".
• Define surface contact between the wheel and ground before generating the mesh.
• Define bonded contact between the wheel and axis before generating the mesh. (this will force the mesh to match)
• Generate the mesh.
• Define surface contact between the wheel and axle.

Another option would be to add a little bit of space between the wheel and the ground. This would prevent the mesh from "stretching" in an attempt to match the meshes. In the surface contact settings for the wheel to ground contact, define the contact distance to be equal to the space that you added between the wheel and ground. Essentially, you are using the contact to "fill" the space between the parts in the model.

[Anonymous]

Hello,

This option indeed exists and the solution you propose does work out ;

thank you very much for your answers ,

Marie Malafosse