cancel
Showing results for 
Search instead for 
Did you mean: 

Contact problem in SOL 601/106

Experimenter
Experimenter

Hi all,

 

For my master's dissertation, I have to model a  road tunnel construction in Siemens NX 11.0. I'm a beginning Siemens user.

 

Three tunnel rings are in contact with each other (surface-to-surface contact) as you can see in the attachment. A thrust force is applied, also soil and water pressure is to be applied later. 

 

The model does run when only surface-to-surface gluing is applied, but when surface-to-surface contact is applied for the circumferential joints, the solver gives the error 'No results are found' after calculation. The f06-file just says:

 

ERROR IN ADVANCED NON LINEAR MODULE
SOL601 FAILED

While running, I also noticed that there is no convergence.

I use a SOL601-106 solver type because bilinear springs are to be applied later on. 

Does anyone has suggestions that can help me in running this model? 

4 REPLIES

Re: Contact problem in SOL 601/106

Siemens Phenom Siemens Phenom
Siemens Phenom

I made a couple changes to the model and solved it successfully with contact.

 

1. The contact faces were abstracted quite a bit. I restored them back to their original state and used the Freeze Geometry command to make sure that remeshing wouldn't abstract them again.

2. I assigned a cylindrical coordinate system to be the displacement coordinate system of all the nodes in the model since it seems that you wanted the node to ground springs to act in the radial direction.

3. I edited the constraint to act upon the axial and theta directions.

 

I think the primary source of your initial problem was that the model wasn't constrained in the rotational direction. 

 

Regards,

Mark

Re: Contact problem in SOL 601/106

Experimenter
Experimenter

Hi Mark,

 

Thanks for your reply! 
The model works so far, now I will continue with multiple rings.

 

Thanks a lot!

 

Kind regards,

Sander

Re: Contact problem in SOL 601/106

Experimenter
Experimenter

Dear Mark,

 

I still have one problem:

Could you please explain to me how you restored de contact face meshes? In the model you solved, the contact face mesh is nicely following its original geometry. I don't manage to get that done in my model.

 

Thanks!

 

Sander

Re: Contact problem in SOL 601/106

Siemens Phenom Siemens Phenom
Siemens Phenom

Sander, 

 

The model as you provided it had faces merged significantly in the contact areas. Each contact area is defined by 2 pads/bosses offset by 5.5mm or so. See the attached JPG. I intended to "correct" each region and represent them as shown in the JPG. I was a bit hasty and didn't get them all like this, but I think they all have at least one side of the contact maintained well from a geometric perspective. That is, the JPG shows all of the faces in the contact region represented in the mesh. None of the faces in the contact region are merged.

 

Your original model had the pads/bosses completely merged out of the model. The 12 eges defining each of these features were removed during meshing. That's because the small size of the pad/boss was less than your small feature tolerance when you generated the mesh. I restored the edges using Split Face, by suppressed edges, then I used the Freeze Geometry command to prevent the pending mesh update to remove the edges again. See the 2nd JPG to see the definition of the Freeze Geometry operation. It actually shows 2 areas that I froze incorrectly. My intent was to freeze only the narrow pad/boss faces.

 

A good practice would be to define a Freeze Geometry feature for the areas you wish to maintain geometry before meshing. Then regardless of your meshing abstraction tolerance, those faces will not be abstracted.

 

Regards,

Mark