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
- Gap as contact

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

10-13-2017 11:22 AM

I am studing the static non linear analysis, this is a simple assembly where I have create a surface contact simulate by gap elements, material is elasto-plastic type, but I am not able to obtain any results. It seems that contacts don't work. Any help will be appreciate.

AMinati

Labels:

4 REPLIES

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

10-13-2017 04:34 PM

The linear analysis fails with the following message in the f06 file:

0

0

GRID POINT ID DEGREE OF FREEDOM MATRIX/FACTOR DIAGONAL RATIO MATRIX DIAGONAL

533 T2 6.01603E+13 1.84200E+06

^^^ USER FATAL MESSAGE 9137 (PHASE1D)

^^^ RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIOS IN MATRIX KLL.

Inspection of the constraints, shows there is no constraint in the T2 or Y direction. You need to constrain this rigid body motion on at least one of the parts to get a solution. Also, your gap elements are using the basic coordinate system and the gap contact direction uses the coordinate system X direction. You need to create an local coordinate system where the X direction is in the contact direction.

Regards,

Joe

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

10-13-2017 05:01 PM

I have updated the model with the correct gap coordinate system, improve the mesh, loads and constraints. In the zip file there is the static solution with contact surfaces and the non linear one. In the non linear I have tried the static solution with gap as contact, but the solution has a lot of difference to the static with contact surfaces and the non linear analysis don't converge. I am waiting for suggestions

Best Regards

AMinati

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

10-17-2017 11:10 AM

I believe the biggest problem are still your constraints. There is still no constraint for rigid body motion in the global Y direction. I do not know how the real structure is supported and reacts the loading, but the deformations based on your boundary conditions do not make much sense to me.

I deleted your gap elements and used linear contact so you can see how your structure is deforming without the nonlinear material effects. The pictures below show how your "piece 2" is rotating about the edge of "piece 1".

A few other things to be aware of:

1) "gaps as contact" is not valid and ignored for sol 106 nonlinear. This is because "surface to surface contact" is not supported in sol 106. The gaps work based on the gap property inputs only. For sliding surfaces, gaps may not be the best choice.

2) Your model is all solid elements except for the gaps. This results in zero stiffness in all rotation dof's(4,5,6). In linear solutions, AUTOSPC removes those zero's for you, but in SOL 106, AUTOSPC is not active and this can cause convergence issues in SOL 106, better to use "permanent constraints" to remove 4,5,6 for nodes for your nonlinear runs.

3) I made a SOL 106 nonlinear with your gaps active, and the 4,5,6 removed via permanent constraints, it converges and the deformed shape looks basically like the linear contact results below.

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

10-18-2017 02:41 AM - edited 10-18-2017 03:12 AM

The constraints are OK! Take a look at the first part: I have splitted the first and the second parts in two so to have congruent mating surfaces and to allow the use of Hexaedral elements.

Contraint Z fix the first part in Z direction, while the second part is fixed in the same diretion by the Gap elements;

Constraint -5° fixes the two parts so that they cannot move perpendicular to this plane;

Constraint +5° fixes the two parts so that they cannot move perpendicular to this plane which is different from the -5°, so all the parts are correctly constrained.

Then I have followed all the suggestions made in the Nastran "Basic Nonlinear Analysis User's Guide", in particular I have used the proper element type, Gap element properties (I move the positions of one part to the other so that Gap element have no coincident nodes), create the correct Gap coordinates system (X direction along the Z global direction), set up the steps to 100, and tried a lot of configurations on "Model, Loads, Non Linear Analysis..." and so on, and finally the model was able to converge! And results are quite similar to those obtained by a static analysis with contacts. See my last model. The problem now is that this was only a simplified model of my analysis and even if I have implement all the solutions used in the semplified model I am still no able to converge the real model.

Best Regards and many thank for the suggestions

AMinati

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc