Contact US

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!

*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

Building contact between two solids

Building contact between two solids

Building contact between two solids


two solid geometries were imported in Patran. Those have different material properties, but have no relative motion to each other. So they should be fixed together. Although there are RBE2 connections by BAR2(1D) elements, but that's not a realistic way to simulate it. So, a CONTACT needs to be established between these two solids.

So far I know, the option is available under LOAD / Boundary Conditions.

**I selected 'deformable bodies'.

** But I am not sure that, I sould select 2D (as the contact surfaces are 2D) or 3D (as both of the solids are 3D TET10 elements).

** Then under 'Input Data', there are some options to define 'Friction Coefficient (MU)' and 'Analytic Contact' / 'Contact Area'/ .... The question is that, if I select 3D, should I define the contact surfaces between two solids here ? (under 'Contact Area')

** Then under 'Select Application Region', should I select solid geometry or 3D TET10 elements? And, should I select both solids, or one solid each time for each contact definition?

It would be a big help, if somebody can help me here. Thanks in advance!

RE: Building contact between two solids

You should use 3D option.
You don't need to select Contact Area.
You should define 2 contact bodies, and select 1 solid for 1 contact body.

After you define 2 contact bodies, in the subcase definition, you can define contact table. And you should deactivate self contact (contact between 1 and 1, and 2 and 2). You need to make contact between 1 and 2 to be glued. You can click on the entries to toggle among empty(no contact), T (touching), and G (glued).

RE: Building contact between two solids

Hi hezhj2000,

thanks a lot for your help. Please let me ask you more about some details.

I defined seperately SOLID1 contact and SOLID2 contact in my database (by selecting the geometry, not by the FEM TET10 elements as you suggested). SOLID1 is fixed with a rotating shaft and SOLID2 is fixed with SOLID1 by nut-bolt joints. So the relative sliding motion between these two solids has been fixed by those bolt connections and at the same time they are mainataining this contact.

I found something useful in the MSC software website and another power-point presentation, but for clarification I need to know something more. The URLs are here:

Now the questions are: (a screen-shot photo attached)

1. Which one should be Master (Touched body)? (SOLID1 or SOLID2) As it is noticeable in the 'Contact Table' that, one should be Master and another should be Slave.

2. Which option should I select, 'Touch All' or 'Glue All'?

3. In 'Contact Detection', Automatic / Double SLided / 1st->2nd / 2nd->1st ?

4. What about those other options? Do I need to define those or should I just keep it as it is? (e.g, Retain Gaps / Stress-free Init Cont / Delayed Slide Off / Allow Separation / Retain Moment / Distance Tolerance / Bias Factor / ...)

5. I need to export the whole database as a BDF file. Because later I have to import it in a specialized preprocessor of NASTRAN for further calculation. For exporting it as a BDF, should I go by the options Analyze> Entire Model > Analysis Deck > Subcases (contacts have been defined here) > Apply ? (I meant, will all of those contact parameters be exported along with the BDF file?)

6. Also, should I define the solution parameters as per this suggestion?
"Secondly, if you are using higher order elements like TET10s, you need to change the following:
In Analysis>Solution Type>Solution Parameters>Contact Parameters>Separation>Separation Criterion, tick the box Stresses as opposed to Forces. Then in Analysis>Solution Type>Solution Parameters>Contact Parameters>Contact Detection, click the Activate Quadratic Contact box."

I am looking forward to have a reply from you. Best wishes!

RE: Building contact between two solids

1. usually contact body with finer mesh and softer material should be the slave.
2. from you description, the contact between the 2 bodies is touching contact.
3. These options determines the mater/slave. If you are not sure, you should use Automatic.
4. You should read Nastran Quick Reference Guide to get an idea about what these parameters are, and decide what to change. Usually 'Distacne Tolerance' is something we need to keep an eye of.
5. You can search 'BCTABLE' to see if the contact has been output.
6. If you are using TET4 elements, no need to do that. If you are using TET10 elements, yes.

RE: Building contact between two solids

Hi hezhj2000,

Thanks a lot for your answer. I am busy finishing some works right now. I will contact you later with more questions if I have some. Please don't get bothered smile

Till that time! Have a nice time! smile

RE: Building contact between two solids

Hi hezhj2000,

I am going to bother you again now. wink

I performed the calculation as Linear Static, and first time it failed. The reason seemed to me that it needs SOL600. So later I choose SOL600 under 'Linear Static'. Do you think it's a correct way of analysis?

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! Already a Member? Login


Low-Volume Rapid Injection Molding With 3D Printed Molds
Learn methods and guidelines for using stereolithography (SLA) 3D printed molds in the injection molding process to lower costs and lead time. Discover how this hybrid manufacturing process enables on-demand mold fabrication to quickly produce small batches of thermoplastic parts. Download Now
Design for Additive Manufacturing (DfAM)
Examine how the principles of DfAM upend many of the long-standing rules around manufacturability - allowing engineers and designers to place a part’s function at the center of their design considerations. Download Now
Taking Control of Engineering Documents
This ebook covers tips for creating and managing workflows, security best practices and protection of intellectual property, Cloud vs. on-premise software solutions, CAD file management, compliance, and more. 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