MSC Nastran Contact Analysis Suggestions

[VN1981]

Hello,
We have to develop FE methodologies for our internal purposes as well for a client. We primarily use Femap with NX Nastran, but in this case, the client has asked us to develop methodologies for MSC Patran/Nastran.

Anyways, one of the cases involves solid contact. Particularly, a pin subjected to double shear.

Initially, the exercise was carried out in Femap by a colleague and after a few tries, we were able to obtain good results i.e. the deformation pattern looked realistic!

I am trying to do the above using MSC Patran and I am completely stuck. I can run the analysis successfully, but the output i.e. deformation pattern is no where as elegant or realistic like the output obtained using Femap. I know the contact parameters in NX Nastran vs MSC are slightly different and thus the confusion or roadblock!

I am posting screenshots of my contact table settings etc. I am using SOL 101. The MSC Patran version I am using is 2016. I would appreciate some pointers on how to proceed from here.

Analysis Setup:

Deformation output from MSC Nastran

Deformation output from NX Nastran

So far, here are the different changes I have carried out.

1. Enabled Initial Stress Free Condition (ICOORD = 1)
2. Enabled Augmentation to Automatic in Segment-Segment Contact.
3. Tried increasing ERROR to 0.02 and BIAS to 0.95.
4. Based on a couple of papers, tried designating the solids as "Analytical Body Contact "(ISDPL) in BCBODY. But the analysis did not terminate even after 4 hours of run. Monitored the F06 file for any errors, but nothing appeared. Finally, I had to terminate the analysis. In NX Nastran, the analysis was done just shy of 20 minutes.

I haven't played with any of the penalty parameters and/or penetration. They are set to defaults.

Even with all the different changes, I am getting the same deformation pattern.

 

[Regretful]

Is there some sort of thickness added to the surface of the solid elements that causes penetrations?

Also, if i am not mistaken SOL101 is a linear solver and this problem looks like it could be non-linear.

Good luck

 

[VN1981]

I am applying 100 lbs total load. The thickness of each plate is 1" and the pin dia is 1". I think there is very little chance that the problem can be non-linear. NX Nastran solved the above problem using SOL 101.

Nope, as far as I know, the mesh is completely of solid elements. No surface elements of any sort. Also, there are no penetrations as far as I can tell.

 

[dmapguru]

Hi,

These displacements looks spurious. Did the model converge to full load?

I see you have a friction coefficient defined, which is good because this is the only thing that will stop the bolt rotating in the hole. However, did you activate the friction type in the Analysis -> Solution Type -> Solution Parameters -> Contact Parameters -> Friction menu? You should set the Friction type to Coulomb. This will result in the BCPARA,0,FTYPE parameter being set to 6 in the Nastran input file. Without this parameter, your friction is not active.

You should also try setting the LCNT line option of NLSTEP to 1; by default, linear contact will apply the load in 10 equal steps, 0.1*total load at a time. The job is quasi-linear, so try setting LCNT to 1.

If this checks out and you still can't get things working, post the Nastran input file and I'll take a look.