## General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

#### Nonlinear analysis convergence issues

• henriquegpo
Subscriber

I am trying to simulate part of a system which works under high pressure (1GPa). I am using a 2D axisymmetric model for that:

I've fixed the model in one edge that should represent the threaded connection to an external fixture device and applied pressure on the edges up until where the sealing (not represented) should act. Axis of symmetry is on the bottom edge of the smaller part. Contact between the parts is frictionless.

Both parts are from stainless steel (DIN 1.4542) hardened to H1050 condition (yield strength = 1140 MPa and Tensile Strength 1210 MPa). As the manufacturer could not provide me a strain stress curve, I am using a bilinear hardening model, with a tangent modulus of 512 MPa (extracted arbitrarily from literature).

The problem is that the simulation converges very well until the very last iteration, where suddenly some elements become highly distorted (usually near the contact regions with radii). I tried tweaking the settings with everything I could: intense mesh refinement, improved contact settings, several substeps, etc. I don't know anymore how I could fix that. My idea is that it this behavior is probably related to the material model, but I can't explain exactly why this would happen.

I attach here a link for the archived project, in case anyone would like to try it out.

I would appreciate any insights from you. Thanks in advance!

Henrique

• John Doyle
Ansys Employee

Two questions:  Does it converge without the BISO plasticity included?  If yes, is the plastic strain very local or thru an entire section.

If thru an entire section, the non-convergence could be indicative of a physical instability (i.e. part will yield and break under this load and with this material).  If plastic strain is very localized, perhaps it is fictitious.  Sometimes a coarser mesh is helpful or adding a more generous radius (if applicable).

If it does not converge, even with no plasticity included, the source of non-convergence is something else, perhaps contact is insufficiently scoped or pinball is too small, but it depends on the feedback in solver output.

• henriquegpo
Subscriber

Yes, the model converge with linear material properties.
The plastic strain is high, but somewhat localized. I show you the regions the following pictures:

Near the contact region:

"Near" the fixed support:

Here is also the unconverged stress plot:

In real life I would expect some plastic strain indeed, especially in the contat region, resulting in something like an inprint of the smaller part on the larger one.

In the solver output I see some warnings of "convergence has been achieved in spite of large penetration" during the substeps 1 and 2 (probably because I reduced the contact stiffness with a factor of 0.1). After that, I see messages of "too much penetration" but not this same "convergence in spite of large penetration" as in substeps 1 an 2.

Than in substep 19 (I set it to 20 this time, but tried with 200 also) I got 2 errors that a couple of elements became highly distorted. And the non converged deformation plot shows the deformed elements exactly where the plastic strain occurs near the radii in the contact region, but not exactly in the radii. Actually where the small part has a radius, the bigger one distorts, and vice-versa.

I'll try a larger radius, even though I believe it would no be possible in the design.

Any other ideas?

• peteroznewman
Subscriber

How is it possible for the pressure to suddenly end in the middle of the side of the part?

What is the true nature of the boundary condition on the top horizontal edge? Why is a Fixed Support a good approximation to the true boundary condition?

• henriquegpo
Subscriber

Hello Peter,

Here is an image of the complete CAD model (already a bit simplified):

The pressure is built from this big vertical bore, coming from the bottom. In the FE model I’ve considered that the pressure is applied to the surface of the pink part until the point the sealing acts, including the region where the sealing parts (black, orange and yellow) are in contact with the pink one. I am not interested in simulating the sealing behavior, and although I know that the pressure itself will vary a bit in that region, I thought that it would be a reasonable estimation to apply it uniformly up to that point.

As for the fixed support, the pink part is screwed to this light-blue outer part via a M30 thread. I thought that it might also be reasonable to consider it completely fixed.

Do you think that the boundary conditions could be better represented? I am eager to hear your suggestions.

Best,
Henrique

• peteroznewman
Subscriber

Hello Henrique,

Thank you for the details!

I have built O-ring seal models to determine if the O-ring will succeed in making a seal. The seal works if the contact pressure of the O-ring is greater than the fluid pressure. Otherwise, the fluid pressure would penetrate the seal. The contact pressure ends where the seal ends, and that appears to be where you ended the fluid pressure, so it looks like you have made a reasonable idealization.

The M30 threads have radial clearance and the contact face on the thread has a 30 degree angle relative to the X axis (which is vertical in these screen shots). A more accurate model would be to include the thread geometry.  A simplified boundary could be to use a Displacement of Y=0 and leave X=Free so that radial deformation can occur. Once the model converges, you can see if this makes a better boundary condition than a Fixed Support.

It sometimes helps the solver converge if, under Analysis Settings, you turn on Auto Time Stepping and change the Maximum Substeps to a large number like 2000.  It will only use them if it needs to, but if you limit it to a small number, convergence may fail. In your case, it didn't need that, but it is a best practice to do this.

You created a good quality mesh. I opened your model on a computer with the Ansys Student license installed, so I can't solve your model with the mesh you created as it exceeds the student node count limit of 128,000 nodes.  I changed the Element Order from Program Controlled to Linear and the node count went down to 43,000 nodes.

To diagnose why convergence fails, click on the Solution Information folder and type a 3 for the Newton-Raphson Residuals and type a 3 for Identify Element Violations.  When convergence fails, first look at the Solution ouput and scroll to the bottom to find the first ERROR.  In this case it says a highly distorted element.

Click on the HDST_Elements plot to see where the highly distorted elements are located.

During the solution, the shape became worse.

The corrective action is to make a better quality element shape in the mesh before solving. I made much larger elements and made sure the inflation layer had layers that would cover the region of concern.

Now the model converges.

If you add the thread geometry back on the plug and include frictional contact with the female threads on the part with the hole in it, you will see the stress in the threads be distributed over several threads and the stress concentration from the Fixed Support will be reduced.

• henriquegpo
Subscriber
Hi Peter,

I would like to once again thank you for such fruitfull insights. Also thanks to the other colleagues for the help!

I manage to get the analysis to converge following what you said: coarser mesh and auto substepping. I have also tweaked a bit more the contact definition, making use of Normal Lagrange formulation, Nodal-Projected Normal from Target detection and Flipping contact/target edges.

There are a few further questions I would like to ask:
1. I am not entirely sure why a coarser mesh is helpful. I thought that, if the elements had a decent aspect ratio (square elements), than the size itself would impact mainly on the “resolution” of the analysis. What I am imagining here is that, as this is a nonlinear material model, when the plastic strain reaches a certain limit, the tiny elements cannot keep its shape, therefore bigger elements would perform better. Is that correct?

2. I would like to have a somewhat decent stress evaluation from that model, especially around the contact interface. Using a coarser mesh can sometimes lead to a non-uniform stress distribution plot. So this seems to be the case that a compromisse between being able to simulate and exctrating accurate stress results must be make, right?

3. I am not yet at a point that I would like to include the thread geometry in the model, but I would like to have an estimate of how much force would rise at the threads in this condition. Is the force reaction from the fixed support a good estimation?

Still on mesh size topic, I tried to reduce it to see what would be the lower limit with which the simulation would still converge. I noticed that there is an intermediate limit, from which the simulation still converges despite of errors popping up. The error was of highly distorted elements, leading to bisection. And there are also notes of the incremental plastic strain being larger than a criterion, also leading to bisections:

Are the simulation results still valid on that case (convergence achieved despite errors leading to bisections)? Is there any aspect I should keep an eye on when that occurs?