Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here


MSC Nastran Contact Analysis Suggestions

MSC Nastran Contact Analysis Suggestions

MSC Nastran Contact Analysis Suggestions

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.

RE: MSC Nastran Contact Analysis Suggestions

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

RE: MSC Nastran Contact Analysis Suggestions

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.

RE: MSC Nastran Contact Analysis Suggestions


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.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


White Paper - Effects of AIA Quick Guide to UL 489 or UL 1077
The function of a circuit breaker is to provide overload (thermal) and short-circuit (magnetic) protection to a circuit and its downstream components. A circuit breaker functions like an airbag in a car, protecting circuit components and people by tripping the circuit to interrupt the current flow if it detects a fault condition in the control system. Download Now
White Paper - Guide to Integrate Large-Format Additive
As with any new technology, getting into large-format 3D printing begins with investigation. The first question may be a simple one: what does “large-format” mean? For 3D printers, “large” is a relative term. Many extrusion-based (FFF) 3D printers are referred to as desktop machines, because they fit on table space. Some of these have very respectable build volumes – but when it comes to “large-format,” the machines will need their own dedicated floor space. Large-format 3D printers have significant build volumes and are most often found in professional settings, like manufacturing facilities and R&D centers. Download Now

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close