Building contact between two solids 2

[Xenon2014]

Hello,

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!

 

[hezhj2000]

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).

 

[Xenon2014]

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:

http://www.mscsoftware.com/training...Structural/nas_run_forms.04.09.html#ww1016551

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."

http://www.eng-tips.com/viewthread....ewthread.cfm?qid=326477&tmac=fav&val=1,326477

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

 

[hezhj2000]

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.

 

[Xenon2014]

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

Till that time! Have a nice time!

 

[Xenon2014]

Hi hezhj2000,

I am going to bother you again now.

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?