Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

Non linear analysis with contacts - Solution issues and advices

Good evening all,

I have tried to perform a structural analysis involving a pin and a slot.
I have set up a Non Linear analysis with contact using small displacement (NLPARM).
At the beginning the pin is not touching the slot, then It touches the slot and the contact start working.
On the pin acts a LOADADD force (Fx+Fz), the other dof are blocked (rotations and traslation along y). Otherwise the slot is fixed (only traslations, no rotations because I think is unuseful).
Attached you can find the model (Hypermesh 2017.2 model).
I have set up a contact with a property type SLIDE and Discret N2S.
Furthermore I have chosen the pin as master and the slot as slave.

The problem is that after a bit it comes up with a result message (analysis completed), but it seems It hasn't performed all the increments I have set up. I think the results have not any sense.

Could you please take a look at the model? Is that solution correct??

Furthermore, there is attached a screenshot of the run panel of Optistuct. In the upper right corner threre are the Iterations column and the Subcase column. I'm not able to understand why the Iteration or Subcase are not matching the number of increments I have set up (30).
What are Non_EUI_st, GapClose_st, etc..??

Do I need to change contact parameters adding, for example, a contact property?

Many thanks you very much for the your help and time

<?xml version="1.0" encoding="UTF-8"?>

Unable to find an attachment - read this blog

Find more posts tagged with

English

OptiStruct

Accepted answers

All comments

Adriano_Koga

you should take a look at the .out file as it gives you a better understanding of what is going on with each load increment.

In the newer versions you can especify exactly how many increments are going to be stored into the H3D results.

In the past, it was not possible to guarantee that you would have exactly 30 steps in your results, as the solver could 'speed up' at some point and run in fewer increments.

Depending on how large the displacements in your model, you might need to activate LGDISP and under contacts you might need FINITE SLIDING.

Staedtlerp

Thank you very much @Adriano A. Koga
I think I have sorted out the problem. The main problem was related to the PARAM/EXPERTNL/CNTSTB bulk data; it was not activated. Then, I looked for a solution on this forum and I find something similar to the issue I encountered. Now It goes straight with no problems.

What do you mean with FINITE SLIDING?? is it mandatory to activate it for LGDISP analysis??

Thank you very much

Furthermore, I'm not able to understand what are Non_EUI_st, GapClose_st, etc.. yet. I don't find anything in the online guide.
Could anyone explain this?

Thank you.

Adriano_Koga

You might want to take a look at this video here:

https://www.altair.com/resource/finite-sliding-analysis

Essentially, the default behavior of contacts is Small Sliding, where the contacts are assumed to have very small sliding between the parts, so that the contact pairs (master and slave) can be considered the same for the whole analysis.

For Finite and Continuous Sliding, the sliding between the parts is larger, so that one part slides over the other, and the contact regions change all the time.

The classical example is a rack and pinion assembly.

For this kind of contact, the contact paris (master and slaves) need to be updated every time, so that the new contact pairs are found.

The difference between finite and continuous is just the frequency that this update occurs. Finite updates the contact pairings at each load increment. Continuous updates it at each iteration inside the increment.

These are computacionally more expensive that small sliding, but for some cases they need to be used, otherwise the model might fail due to the change in contact pair, or if the contact distance increases too much, and the master 'loses' the slave node of its sight.

Staedtlerp

Thank you very much @Adriano A. Koga for this explanation, it is very helpful. I've never used these type of contact (finite or continuos sliding) before; I've never had to use it because my simulations involve essentialy small sliding between parts. I believe it will be very helpful for me in the future. Thanks a lot/emoticons/default_smile.png' srcset='/emoticons/smile@2x.png 2x' title=':)' width='20' />