SOL 400 contact problem, where in SOL 601 is OK

[jacksonfem]

Hello,

I have a model with solid elements, simulating a clip, as you can see in the image below. In SOL 601, with NxNastran, I can easily simulate the male clip moving out from the female and in again with a transient analysis, as you can see in the images sequence. But when I try to perform the same simulation is MscNastran's SOL 400, the solver cannot find convergence and stops. The non-convergence begin when the 2 bodies are in contact. I really can 't find why. I don 't use any special contact parameters in SOL 601. Just the defaults.
In SOL 400 I use adaptive time stepping and not fixed, just like in SOL 601.

Do you have any idea of what is happening?

 

[aerostress82]

My guess would be that between SOL400 and SOL600, the main difference is adaptive meshing-which means if an element is too much warped, it will be "remeshed" to get rid of the bad quality (thus the numerical errors).
Could you share the Nastran deck with only the headers and boundary conditions for both SOL400 and SOL600 as 2 separate text files? (exclude the element and node cards only please).

Also try to include NLSTEP and similar cards (except element and node cards - only pure boundary conditions and Nastran headers, groups/sets & DMAP parameters is what I'm looking for) regarding both the SOL400 and SOL600?


It would be interesting to compare the 2 decks as 1 is with adaptive meshing and 1 is not. It could also help with the understanding of your SOL400 analysis setup if your problem "isn't" adaptive meshing - but smt else.

Spaceship!!
Aerospace Engineer, M.Sc. / Aircraft Stress Engineer

 

[jacksonfem]

It 's not SOL 600. It's SOL 601 of NxNastran (by ADINA). I always worked for nonlinear contact problems with Femap and SOL 601. Almost everything I did could be easily solved. Then I start using MSC's SOL 400...as the original one. But in some contact problems, it just not converged...Also, I don't use adaptive mesh...

Below a typical MSC Nastran SOL 400 file (from many that I have tried)...

-------------------------------------------------------------------------------------
SOL 400
CEND
ECHO = NONE
SUBCASE 1
ANALYSIS = NLTRAN
TSTEPNL = 1
SPC = 1
LOAD = 1
DLOAD = 1
BCONTACT = ALLBODY
DISPLACEMENT(SORT2,PRINT,REAL)=ALL
STRESS(SORT1,PRINT,REAL,VONMISES,CENTER)=ALL
SPCFORCES(SORT2,PRINT,REAL)=ALL
NLSTRESS(SORT1,PRINT)=ALL
BEGIN BULK
PARAM,LGDISP,1
PARAM,POST,-1
PARAM,AUTOSPC,YES
PARAM,GRDPNT,0

BCBODY 1 3D DEFORM 1
BCBODY 2 3D DEFORM 2

BSURF 1 ................
BSURF 2 ..................

BCTABLE 1
SLAVE 1 0. 0. 0 1
1 0 0
MASTERS 2

MAT1 3 1960. 0.3 1.5-5 1.+0008D08
+0008D08

TSTEPNL 1 10 0.3 PFNT PV
.100
0

TLOAD1 1 1 1 1

TABLED1 1LINEAR LINEAR +0008D1A
+0008D1A 0. 0. 0.3 0.1 0.6 0.2 0.9 0.3+0008D1B
+0008D1B 3. 1.ENDT

ENDDATA
--------------------------------------------------------------------------------------------------


And below SOL 601 file...
------------------------------------------------------------------------------------------------------
NASTRAN SYSTEM(442)=-1, SYSTEM(319)=1
ASSIGN OUTPUT2='advnlin.op2',UNIT=21
ID Clip,Femap
SOL 601,106
TIME 10000
CEND

BCONTACT = ALLBODY

TITLE = clip_unclip_Dimitris.nas
ECHO = NONE
DISPLACEMENT(PRINT) = ALL
STRESS(PRINT) = ALL
BCRESULTS(TRACTION,FORCE,PRINT) = ALL
SPC = 1
DLOAD = 107
TSTEP = 109
BCSET = 108
BEGIN BULK
PARAM,LGDISP,1
PARAM,POST,-1
PARAM,OGEOM,NO
PARAM,AUTOSPC,YES
PARAM,GRDPNT,0
NXSTRAT 1 AUTO 1 NPOSIT 1 LSEARCH 1 +
+ ELRESCS 1 ELCV 0
DLOAD 107 1. 1. 101
TSTEP 109 50 .2 1
MAT1 3 1960.753.8462 .3 1.5-5 0. 0. 1.
TABLED2 1 0. +
+ 0. 0. 3. 1.ENDT
TLOAD1 101 102 DISP 1
BCRPARA 1 0. FLEX
BSURFS 1 .................
BCRPARA 2 0. FLEX
BSURFS 2 ................
BCTSET 2 1 2 0.
BCTADD 108 2
ENDDATA
-------------------------------------------------------------------------------------------------

 

[aerostress82]

Below may be the possible solutions to your SOL400 analysis:
[ul]
[li]TSTEPNL 1 10 0.3 PFNT PV (not sure about the exact format of this card as I mostly used NLPARM for nonlinear static analysis with contact only - but you might wanna look into TSTEPNL card from MSC Nastran Quick Reference Guide and pick a different format of this card where EPSU and EPSW are defined as values lower than the default -0.01 value (ie. -0.1).[/li]
[li]You don't seem to have your DLOAD card in your SOL400 analysis. It is defined in the header, but then in the rest of your Nastran cards, I can't see a DLOAD assigned as it was assigned in SOL600.[/li]
[/ul]

If I had Nastran at home, I could get the original complete analysis file for SOL400 from you and get it working, but it doesn't seem possible.
Please let me know if the above possible solutions don't help with your case.

Also please copy paste your FATAL errors if you can for SOL400. That also helps a lot. If you can get this to work in MSC Nastran SOL400, it will be worth your while as from what I've received in Beta testing of Patran/Nastran 2016, things are gonna get a lot easier and will be less time consuming for the future as well. Try to get your MSC Nastran working for your cases, you'll be grateful for it in the future.. All the Best!





Spaceship!!
Aerospace Engineer, M.Sc. / Aircraft Stress Engineer

 

[jacksonfem]

1) I used TSTEPNL because it 's a pseudo-transient analysis (3 seconds duration, so the inertia effects have no meaning), cause I didn 't want to do it as a static with steps.
2)TLOAD is the correspondence to the DLOAD

I didn 't find a reason so I tried to do a static analysis with step. And I want your help, because what is happening, it doesn't seem logical to me...
So, let's start:

STEP 1: Force on the male clips (OK!)

https://app.box.com/s/9a12b74ybqbqlwvir6v0ieyzgur8efrr

STEP 2: A little displacement for the male with the force of step 1 steady (OK!)

https://app.box.com/s/xrr3idz7fdlcziyps4qy7lumg3b47r8t

STEP 3: Unload the clips to touch the female (PROBLEM!)

https://app.box.com/s/a254y1kxg2ljook4tn85k9cehoxiplld

STEP 4: A large displacement for the male to the final displacement (OK!)

https://app.box.com/s/9279qecfnju9bp24nbgwymc3x7dmipiy

STEP 5: A step without any load to return it to it's initial position (PROBLEM!!!)

https://app.box.com/s/h1nwezx4a6d8qou1i1oepgfc6eg7tu7e

I can't understand why is happening this. Something with the contact is wrong. I only set BCPARA, bias=0.99 and error=0.005

With the same contacts, the SOL601 in NxNatran works fine.

 

[jacksonfem]

And the crazy thing, is that when I modify the model and the initial position of the male is out of the female and i just move it, it's all working fine!!

https://app.box.com/s/tkbmcs3ay0wjg1b956ov85fom22qleia

 

[aerostress82]

Regarding what you said last that it is working the other way around, your problem is most definitely a convergence issue due to the epsilon values. Plase refer to my first reply above about the EPSu and EPSW values in your TSTEPNL card. It should most probably solve your problem. Please read comment 1 in that post and check the Nastran Quick Reference Guide on how to implement those cards into it.. Let me know if you solve it.

Spaceship!!
Aerospace Engineer, M.Sc. / Aircraft Stress Engineer

 

[jacksonfem]

OK, I'll try, but I would not be happy if it could be solved by adjusting the convergence ratios in so "big" values. A value of 0,01 it's not a promising value for a reliable results. Also in addition to SOL601, where the solution is very easy with pretty small convergence ratios.

I will try and feedback!

 

[jacksonfem]

I did it with convergence ratios been equal to 0,1. Try both with NLPARM and NLSTEP. It's not working again. The same behavior as before. The problem is that for some reason, the contact in some steps is behave as glued contact...if you see the videos it's clear.

 

[jacksonfem]

Finally I find it. The problem was that the master and slave sets, where defined by the solid facets of the elements that come in contact. In the file that works fine, the master and slave sets include the whole solid elements and not the only the facets that come to contact. I don't why this happens. With other solvers (LS-DYNA, PAM-CRASH) I don't have this problems with the solid facets.

Thank you for your time and help!

 

[aerostress82]

The reason to why this is happening "maybe" that MSC Nastran was actually created as a linear solver by NASA at the very beginning.
Then they added the non-linear solvers and everything after which helped the non-linear cases to be solved.

It is a linear solver mostly and for plasticity they have MSC Marc.

LS-DYNA and PAM-CRASH (and RADIOS) are the new kids in the game and that's why they were already compiled for non-linear cases like yours.

Where there is "giant" (large) amounts of displacements (mostly an assembly like yours), you will need to go proper with solvers like LS-DYNA and PAM-CRASH. Likewise NX Nastran is going to help as it was created after MSC Software had to give away its MSC Nastran's source code due to no other competition in the market (a couple years ago). So, NX Nastran was created after.

It is actually really amazing that you could fix this issue for MSC Nastran with such small effort. Which version of MSC Nastran were you using? As you mentioned SOL400 I'm assuming you have one later than 2012 as it came into the SOLVERS family sometime in 2013. But exactly which version is it?


As I mentioned in my previous post, (I know this from a manager in MSC software) that they will revolutionize so many things with new MSC Nastran versions. If you have to use NX Nastran, continue using it, but you never know when MSC Nastran will take over. It may be real soon. They "now" understand what they have been lacking in the last 10 years (despite the trustworthiness in industry), and they have been fixing it in the last 2-3 years - but especially they will do more and more by and after the version 2016..

Spaceship!!
Aerospace Engineer, M.Sc. / Aircraft Stress Engineer