turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- 3D Simulation - Femap Forum
- Friction as a Constraint

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

10-18-2015 03:03 PM

FEMAP users,

Quick question for the experts. I've notced that Friction in SOL101 does not stabilize models as expected. I understand that using friction as a constraint is bad practice in Nx Nastran, but I come from the world of ANSYS and this is common practice in both linear and non linear solutions. I've set-up a simple model to demonstrate this issue, and attached images to this post.

This model is a tube placed inside a plate that with center hole. The plate is loaded axially 200 lbs (Y-axis), as well has a small side load 5 lbs (Z-Axis). The friction is used to stabilize model from the side load.

I have run the model in ANSYS as well as Nx Advanced non-linead, and both accuratly predict that friction will prevent the plate from sliding on the tube. However it appears that frction provides no model stability in Nx Nastran. If anyone has some idead I would really like to understand how friction is working in this model.

Thank you FEMAP and Nastran experts!!!

JP

7 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

10-18-2015 05:03 PM

FEMAP team,

One other comment the ANSYS analysis and Nx-Adavanced non-linear analysis were both solved with large defection turned off.

Thanks

JP

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

10-18-2015 07:12 PM

Dear John,

Please share your FEMAP models for linear contact using NX NASTRAN (SOL101) and ADVANCED NONLINEAR (SOL601) to see the details of the analysis, without the models in hand is difficult to know the analysis setup, then comparison is impossible.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

10-18-2015 09:16 PM

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

10-19-2015 06:59 AM

Dear JP,

Your FEMAP model has some inconsistencies, to name:

- You have used
**CHEXA 20-nodes high-order parabolid elements**, good: In contact analysis is critical that midside nodes to reside in the surface geometry, but in your model is located simply in the straight line between corner nodes. I have updated the mesh in both tube & plate to project all midside nodes to geometry (**MODIFY > PROJECT > NODE**), this will avoid to have undesired penetration between meshes, and then hot spot results (you can play with INIPENE to solve the problem as well, but is better to have a correct mesh, see https://iberisa.wordpress.com/2012/01/14/mejora-de-resultados-de-contacto-lineal-con-inipene-en-fema... - The contact definition of SOURCE & TARGET REGIONS is wrong, I have reversed: SOURCE should be the smaller region, ie, the plate.
- You have defined symmetry constraints using global coordinate system, not need at all to use features like "
**SYMMETRIC**", this will create internally local coordinate system. - As a result of the above you have a problem with local coordinate systems: most nodes have assigned local output coordinate systems #3, #4 instead global cartesian #0. Solved using "
**MODIFY > UPDATE OTHER > OUTPUT CSYS**" and assigned to all nodes of the FE model the**0..BASIC RECTANGULAR**.

The critical point here is the **LINEAR CONTACT PROPERTY**: I have reduced the tolerance in some points like **Force Convergence** or **Convergence Criteria method**, but the important point here is the **INTORD = 3** parameter used: **it determines the number of contact evaluation points for a single element face on the source region**. The number of contact evaluation points is dependent on the value of INTORD, and on the type of element face. A higher number of contact evaluation points can be used to increase the accuracy of a contact solution. Inaccuracies sometimes appear in the form of nonuniform contact pressure and stress results. There may be a penalty associated with using more evaluation points since the time for a contact problem to converge may be longer. The table below shows how the number of contact evaluation points is dependent on the element type, and how it can be adjusted using the INTORD option. The “Face Type” column applies to shell elements, and to the solid element with the associated face type.

After setting **INTORD=3..High** (the default is INTERD=2..Medium) I get the following results: contact convergence is achieved is less than 30 iterations, and displacement results are consistent with the applied loadings.

^^^ ^^^NUMBER OF CONTACT STATUS CHANGES: 0 (NCHG:0) ^^^NUMBER OF INACTIVE CONTACTS: 1704 ^^^NUMBER OF STICKING CONTACTS: 300 ^^^NUMBER OF SLIDING CONTACTS: 26 ^^^ ^^^CONTACT ITERATION CONVERGED

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

10-19-2015 08:19 PM

Dear Blas,

Thank you for all of your help. Unfortunetly my model is converging on a different solution than the one you recieved. I have made the following changes to the model.

1) I have updated the nodes to reside on the surface geometry.

2) I have updated my contact surfaces so that the source is now on the smaller mesh region (region 2).

3) I have updated the Convergence Critera to 0..Number of Changes

4) The Force Convergence Tol has been set to 0.005

5) The initial Penetration has been changed to 0.00 Calculated

6) The Eval ORder has been chaged to 3.. High

7) Max Contact Search Dist has been set to 0.5

8) The Out-out coordianet systems had been changed to the Global System for all nodes?

I'm currently running FEMAP 11.1. Has the contact been changed in NxNastran10, because my results look very differnet from yours?

Again thank you for your help and expertise.

JP

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

10-20-2015 11:30 AM

Blas and FEMAP experts,

I'll download the new FEMAP 11.2.2 with Nx Nastran 10 and re-run this model. Otherwise I believe I have a something that is producing erroneous results in my model.

Thanks

JP

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

10-20-2015 07:25 PM

Dear JP,

The Ouput CS#5 & #6 still are alive. You have a lot of nodes that still are associated to local output coordinate systems, see below. Use **MODIFY > UPDATE OTHER > Output Csys > select ALL nodes** and assign the **0..BASIC RECTANGULAR.** Next use** FILE > REBUILD **and you will be able to delete all local CSsys.

Revising the SOURCE REGION on the plate you have NEGATIVE SIDE selected: this is wrong!!. The same happens with the TARGET REGION on the tube (**!!??**). Simply I select REVERSE (**Please note I told you to REVERSE the CONNECTOR, not the REGIONS!!**).

I created the HEX20 mesh again and results seems reasonable.:

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc