Learning Forum

[pramod1314]

Hello Everyone

I have got a stress singularity issue at a sharp corner. If I refine the mesh stress increases and doesn't converge.

I added a small fillet at the corner; however that did not help.

I would really appreciate if someone can tell how to deal with these kind of problem?

Thank you in advance.

This 2D-axisymmetric model. Pressure applied from top, bottom fixed, Frictional contact(0.15).

[peteroznewman]

You got rid of the singularity when you changed the sharp corner to a radiused corner.
Now you have Hertzian Contact Stress, which is not a singularity. I don't believe the stresses will keep increasing without limit as the element size gets smaller and smaller. I believe you will be able to plot a mesh convergence plot showing a converging trend line.
Please reply with a table of stress versus element size for the model with the radiused corner.
Also, you only need small elements over a small region near the contact point. Sizing with the Sphere of Influence is a good way to get that effect, but you have to create a Coordinate System at the contact point first.

[pramod1314]

Thank you I have used sphere of influence and went to refinement of 0.0005 mm.

This is yet not converging.
Any suggestions what could be the issue here?

[peteroznewman]

Do not change the Radius of the Sphere of Influence. Make the radius at least 2X larger than the distance from the contact point to the location of maximum stress, much like what you show above.
Best practice is to set the element sizes at a constant ratio. For example using a ratio of 2, you can run the following sequence:
.0005
.001
.002
.004
.008
.016
.032
What is the global element size away from the refined mesh? An image of that would be good to see.
Is the plot True Scale? Look at the penetration the contact delivers, it looks excessive. You might reduce some of the noise in the stress by reducing the Displacement tolerance in the Analysis Settings from the default 0.5% to 0.01% and and reduce the Penetration tolerance on the Contact.
What order is the mesh? Change the element order to Linear and run that sequence. Linear elements will also reduce the solution time.
´╗┐If you leave the ruler in your screen grab, that would help to understand the scale of the geometry. What is the blend radius on the corner?
How much precision do you need in the stress result? Is 10% adequate? Why do you need more precision than that?
There is definitely no singularity because for a typical singularity, the stress almost doubles when the element size is cut in half.

[pramod1314]

Thank you for informative insight about stress increase in singularity. Sorry for late reply, It took me some time to do different iterations.
Details:
Order: Linear
Radius of vertex blend: 0.01 mm
Mesh size top surface 1mm, bottom surface 2mm, contact surface other than the corner 0.25 mm, contact at the corner mesh size is varied using parametric study.


Plot is in true scale in the results now.

I have found the penetration in my model. As you suggested i used penetration tolerance option to decrease the penetration but if I go for lower tolerance the stress values increases so I am not sure how much should be the acceptable penetration tolerance or is there any way to find it out? (I used tolerance (as you mentioned in one of your posts) such that penetration is 10^-6 but the stress values were pretty high)
or I can use Normal Lagrange method to avoid this penetration issue? But using Normal Lagrange gives me very high stress.
Result:
1) Augmented Lagrange, penetration tolerance: Program controlled
2) Augmented Lagrange, penetration tolerance: 0.0001 mm


For mesh size 0.004 mm at the corner results would look like this:




3) Normal Lagrange



As you can see stress are highly depend upon penetration tolerance also the formulation method.

I would really appreciate If you can suggest what should be the approach or conclusion I can draw from here?

[peteroznewman]

A good starting point for mesh refinement study would be to have an element size of about 1/10 of the corner radius. Since you have all these sizes already set up, you could simply change the corner radius to 0.4 mm and just run DP0 through DP3 to look at the plot of those 4 points for Normal Lagrange.
Another refinement is to change the Detection Method of the contact to Nodal Normal to Target, assuming the Target is the flat surface.
Did you change the Analysis Settings to request tighter Force and Displacement Convergence tolerances than the default 0.5%?

[pramod1314]

Thank you for the reply.
I have made following changes:
1) Force and Displacement Convergence tolerance to 0.01
2)Detection Method of the contact to Nodal Normal to Target
3) Method: Normal Lagrange
4) I changed vertex blend /fillet radius and also changed the mesh size to keep almost 10 elements in each iteration (as you suggested).

I can see the results are close to each other but the stress values are very high.
Can I trust these values?
Augmented Lagrange gives the value in the range of 700 Mpa if penetration tolerance is program controlled (penetration is 1 % of deformation).

[peteroznewman]

I didn't explain myself clearly enough. When I suggested a 0.4 mm corner radius which would have 10 elements around it at an element size of 0.04 mm, I meant that the 0.4 mm blend radius would remain fixed at that value, while the number of elements would increase around the blend as the element size became smaller and smaller.
This is a Mesh Independence Study. For a fixed geometry, what element size is needed to get a stress result that doesn't change.
Discard the results you have and run a study at a fixed P87 - VertexBlend2 size of 0.4 mm
I also said that mesh independence studies use a fixed ratio of element size. Using the ratio of 2, the element size sequence is 0.04, 0.02, 0.01, 0.005, 0.0025, 0.00125.
That sequence should show the mesh independent value of stress for the Top and Bottom parts at a Vertex Blend size of 0.4 mm.
If you want to see the stress at a smaller Vertex Blend, then you would rerun the study at some other fixed value of Vertex Blend.

[pramod1314]

The length of the contact region is 1 mm. So 0.4 mm would change the design.

What vertex blend radius do you recommend now after seeing the ruler below?

[peteroznewman]

You can start with the current blend radius shown. Start the element size at 1/10 of that radius and divide it by 2 five times then plot those six points.