Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

Contact Penetration

Altair Forum User

@Prakash Pagadala

Hello Prakash,

I am trying to simulate a model with several contacts in Optistruct (Non linear quasi static). The Materials are all linear but with very Little Young Module (40-300Mpa). But there are big Penetrations between sliding parts and the results are not correct.

Contacts with Problem:

ID 16

ID 17

ID 26

ID 27

ID 28

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

I have followed all Solutions in this Forum but it did not work out. I have tried following Solutions:

-Contact type: SLIDE

-Nlparam NINC increase to 200

-CNTSTB load collector and CNSTB Card in Param (EXPERTNL)

- MORIENT= Opengap

-Additional Clearance: 0.1

-String Value>>Adjust>> Auto

-S2S and N2S (Both tried)

-Track INFINIT and Consli (Both tried)

- Symmetric Contact for IP 16 (2 identical contacts with reverse Slave/Master Component)

- PCONT>>STIFF>>HARD

Because the Simulation takes so much time i share the H3D results too.

Thank you so much for your help

P.s: I should mention that this Model with this Material Parameter has been simulated successfully in Abaqus.

Find more posts tagged with

English

OptiStruct

Accepted answers

All comments

Altair Forum User

Thank you for sharing the files. I will check and update you soon,

Altair Forum User

Can you run a large displacement analysis and check the results?

Altair Forum User

Hi @Prakash Pagadala

Thank you for your answer. Yes i tried it too, but results are much worse. Normal displacement acts better than LGDISP.

Altair Forum User

OK,

I have modified the model a little and waiting for the analysis to come out. I will update you soon,

Altair Forum User

@Prakash Pagadala

I have tried 2 new Models with LGDISP.

1. NINC 100

2. NINC 300/ HASHASSM=Yes

Both of Runs have resulted Error:

Maximum number of time increment cutbacks reached.

In not converged results the model explods.

Altair Forum User

LGDISP is not working. I tried the same. I tried after few modifications and I see no penetration but the model doesn't converge for 1st subcase.

I am trying to fix the same and I will share the updated model soon,

Altair Forum User

Thank you so much, Prakash

Currently i am trying a high value of NINC 1000. It takes a week to have the results.

Altair Forum User

Currently i am trying a high value of NINC 1000. It takes a week to have the results.

I think NINC has nothing to do with that.

Altair Forum User

Can you try with N2S and provide a stiffness of say 1e5?

You can try with increasing the stiffness, but that may not give reasonable results.

I will update my finding soon with another modeling change...

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

Altair Forum User

Hi @Prakash Pagadala

I am very thankful for your help.

I will try your idea and update you the results.

Also the results from NINC 500 are out. (The loads are a Little different, but the principals are the same)

There is 2 issues that i found:

First. there is a jump in the Situation of the Geometry between load step 1 and load step 2. (With CNTNLSUB in Load step 2)

it resets some parts of the geometry. I dont know if it causes the contact Problem, in first load step the contacts are functional a Little but it gets worse in load step 2.

End of load step 1

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

Start of load step 2

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

Second. As you can see in the first Picture, the pink part follows the blue part and goes upside ( Just like that it is Stick contact but it is actually slide) and i expected that it stays down.

Here is the Result file (Please ignore the movement of parts at the front, because the pressure was defined in incorrect direction)

https://www.dropbox.com/s/kmekskydyey7eie/R464.h3d?dl=0

Altair Forum User

Hi @Prakash Pagadala

New Update: i tried your idea with stiffnes 1e5 (NINC 100) and the results are so similar to NINC 500 (1 week calculation) but in a very shorter time (10 Hours), which it makes your solution more helpful. The Level of penetration is the same. Not ideal but much better than the initial Situation.

Altair Forum User

Hi Farzin,

It took 2 hrs on my machine with 1E5 stiffness. But my NINC is 10.

Increase stiffness may give good results.

Altair Forum User

Hello @Prakash Pagadala,

New Updates: I have tried a new Setting with LGDISP and the contacts work very good without any Penetration but the Problem is that in Loadcase 2 it does not converge after 60% and the elements beginn to deform incorrectly, i have tried NINC 100 for loadstep 2 and it didn't help. Do you have maybe any Idea about this Problem?

I appreciate your help

FEM:

H3D:

https://www.dropbox.com/s/9e5cllc9r4s1m7p/T54.h3d?dl=0

Altair Forum User

Unfortunately, I am unable to download the files.

Could you please upload the same to my FTP link?

https://ftam1.altair.com/filedrop/~Ce4god

Altair Forum User

@Prakash Pagadala

I sent the files via your Link again

Altair Forum User

Thank you,

I will check and get back to you soon

Altair Forum User

@Prakash Pagadala

Hi Prakash,

i found 2 wrong values in the model that i sent you. Could please correct them:

1- Node Set (ID= 2) ist redundant, you can delete it

2- The material Parameter for Material Meniscus (ID=3) ist E=59 and Nu=0.49

I am so sorry for the this wrong Settings

With Best Regards

Farzin

Unable to find an attachment - read this blog

Altair Forum User

1- Node Set (ID= 2) ist redundant, you can delete it

I have deleted this already and ran the model and it converges to 70%

Let me try with new material values and i will share my feedback soon,

Altair Forum User

Can you update the solver to the latest?

I am using the file with latest solver update and it is through 70% and still running.

Altair Forum User

Hi @Prakash Pagadala

Do you mean with the new E value for Material (ID=3) it is over 70% now?

Which Version ist the latest? I am currently using Hyperworks 2017.0

Altair Forum User

Ok, the University has provided the 2018.0.

I will update you by new results

Altair Forum User

The simulation is stuck at 70% convergence since the last couple of days and I have a .nl h3d which is around 4gb which I can't share right now.

I will check with experts on this and update you soon,

Altair Forum User

@Prakash Pagadala

Thanks a lot for your efforts.

I tried with solver 2018 too.

Loadstep 2 converges till 68% and then stops.

Altair Forum User

Any update?

If not, try with these settings,

Use S2S instead of N2S

Use CONSLI instead of FINIT

Set S1=1.0e-4 in CNTSTB

Add NLADAPT, NOPCL,0 and run in 2018

Altair Forum User

Hi @Prakash Pagadala

Thank you for your update

I tried your Suggestion, and the model converges to 78% (Load step 2)

did you make it till 100% convergence?

If yes, can you please share the Modell (.FEM).

Altair Forum User

Not really,

I am still waiting for the results to come out from 2018 solver.

Altair Forum User

@Farzin After few test cases, I couldn't the see the convergence. I remember you said that the same model converges in Abaqus,
Is the OptiSrtruct deck converted from Abaqus deck?

Is it possible to share the Abaqus deck with us?

Altair Forum User

Hi @Prakash Pagadala

Thanks a lot for your efforts.

Unfortunately, I have no acces to Abaqus Modell. I just received the Mesh and built the model all by myself in Hyperworks. I read a Research, that used the same Model in Abaqus. I used their boundry conditions for my Modell (same Material_same Forces ...). I have no clue about Abaqus convergence Algorithm. /emoticons/default_mellow.png' title=':mellow:' />

I will update you, if i find something new.

Altair Forum User

@Farzin

OK, I just wanted to check if there is anything missing from the model as I see severe element deformation

If you can find the Abaqus model, please let us know or if you can share the research paper details could help to crack.

Quick Links