equal DOF and ZeroLengthImplexContact

[Lei Lei]

Dear STKOteam,

I am currently working on a simulation involving the contact behavior between soil and structures. For this, I have used two different approaches: equal DOF and ZeroLengthImplexASDContact.

I have observed that while the simulation completes successfully with the equal DOF method, it encounters convergence issues right from the start when using ZeroLengthImplexASDContact.

Could you please help me understand why this is happening? Any insights or suggestions for resolving this issue would be greatly appreciated.

Thank you for your assistance.

[kesavapraba]

Hi, if the zerolengthimplexASDcontact element gives convergence issue from the start of the analysis, it should be related to the definition of the element in your model. Please have a look at the following webinar for a detailed understanding about how it works. https://youtu.be/tXA5guozrFU

[Lei Lei]

Thank you!

it should be related to the definition of the element in your model.

I'm facing an issue where the same model fails to converge when the interaction type changes from equalDOF to ZeroLengthImplexASDContact.I’m having difficulty identifying what might be wrong with the parameters. I think the key parameter to focus on is kn. For my analysis, I use the third-order average stiffness of the model, as shown in Figure 1.

figure 1

93e24bc90253e887fc6c5b3754e6463.png (63.59 KiB) Viewed 1956 times

model

f32655ed656b11363eda1abe08c0769.png (87.62 KiB) Viewed 1956 times

Additionally, in other models with multiple analysis stages, including an initial analysis before the tunnel addition stage, the model often fails to progress when ZeroLengthImplexASDContact elements are introduced (Figure 2), or faces a complex root error occurs (Figure 3). In some cases, the calculation even terminates prematurely before entering the stage (Figure 4).

figure 4

f2fff97af8d7eda26859553863fe0ee.png (67.66 KiB) Viewed 1956 times

figure 3

ad4cc4c6789a9a33b84e1285cd0735f.png (84.13 KiB) Viewed 1956 times

figure 2

112e45852b5c5a6645b48e6e669789a.png (80.58 KiB) Viewed 1956 times

Could you help me understand why these errors are occurring?

[STKO Team]

I think the error of complex root comes from a material model.
However, can you share your file to have a look?

[Lei Lei]

Thanks!

My first model is difficult to enter the calculation stage or does not converge very early, and the second model has complex roots.

[STKO Team]

In my case, your first model converges when I remove the -distributed option from the contact. That option is useful when your Kt and Kn are not penalty stiffnesses but real stiffnesses.
However, I see penetration in some places:

contact.png (467.68 KiB) Viewed 1940 times

This happens because you are modeling the tunnel as beams, and the real contact area of the beam is not physically represented. Probably it would be better to model the tunnel with solid elements to properly define the contact surfaces

[Lei Lei]

Thanks！

In my case, your first model converges when I remove the -distributed option from the contact. That option is useful when your Kt and Kn are not penalty stiffnesses but real stiffnesses.

Perhaps the "distributed" option is necessary for beam elements, and defining kn and kt with real stiffness may solve the penetration problem.

However, after several attempts, I noticed that switching from Newton and UmfPack to Krylov-Newton and SparseSYM seems to lead to successful convergence. That said, my results differ from yours by about 5%. I believe there should only be a minor difference between different analysis commands as long as they converge. For my other model, the difference can be as large as 200%.

I've applied this method to a second model, and it worked well.

Do you have any suggestions for choosing the best analysis options?

Best wishes!

[STKO Team]

The only difference can be due to the distributed option that changes the Kn and Kt as a function of the tributary area.
The solver settings can affect the convergence and speed, but not the results

[Lei Lei]

The solver settings can affect the convergence and speed, but not the results

I made a comparison using the complex roots model.

When I chose UmfPack and Krylov-Newton, it showed complex roots. Figure1.

When I chose UmfPack and Newton, it converged and the uy-max was 1.88mm. Figure 2.

When I chose SparseSYM and Krylov-Newton, it also converged, but the uy-max was 5.4mm. Figure 3.

So, which result should I trust?

Figure 1

45dc662e06e715b45e70866e6590fbb.png (93.67 KiB) Viewed 1913 times

figure 2

d239ab3432f0ee29462d07ecae200e7.png (157.71 KiB) Viewed 1913 times

figure 3

bd27c3c753d7d8e4e90f352e27e77a5.png (161.85 KiB) Viewed 1913 times

[STKO Team]

When I chose UmfPack and Krylov-Newton, it showed complex roots. Figure1

This can make sense: A different algorithm (Krylov-Newton vs Newton) can lead to different guess (trial displacement increments) during iterations. If one of them leads to un-realistic trial displacements while iterating for convergence, the material may not be able to solve the constitutive equations (complex roots in your case).

When I chose UmfPack and Newton, it converged and the uy-max was 1.88mm. Figure 2.
When I chose SparseSYM and Krylov-Newton, it also converged, but the uy-max was 5.4mm. Figure 3.

This is strange. While those combinations can give different "paths" during iterations in each step, the converged solution should be the same, because it cannot depend on the stiffness matrix or how it is factorized.

What I see here is that you are using very few time-steps for a problem involving contact.
So there might be 2 reasons for that:
1) You are using a convergence tolerance that is too high, so that also wrong solutions will be accepted
2) You are using some sort of Explicit algorithm (for example IMPLEX in contact), that require small time steps