Showing results for 
Search instead for 
Do you mean 
Reply

Contact in Axisymmetric quad element

When i try to solve an Axisymmetric Quad (under volume) element problem, i get the following error:

** USER FATAL MESSAGE 4690 (SCTEDGE)
GRID POINT 9837 USED IN EDGE-SURFACE GLUE DEFINITION IS NOT A PART OF A SHELL GRID.

I have defined element type as Axisymmetric, with formulation as CTRAX3,CQUADX4,CTRAX6,CQUADX8. 

the contact region output are nodes. 

 

It says EDGE-SURFACE GLUE DEFINITION, where as the connection type is "contact" and i have given an edge-edge connect during regeion preparation.

Still the problem does not solve.

I have attached the file for reference. I have zipped the file.

Could someone please tell me what went wrong.

Thank you.

 

 

3 REPLIES

Re: Contact in Axisymmetric quad element

Dear Sarnath,

Your FEMAP model is not correct, you have a problem with geometry, is not correctly associated with mesh, geometry & mesh is not consistent, if I select nodes from edge#34 used to define region for concrete I see nodes located also in curve edge#110 used to define contact region "fillet plate". I suggest to start again from scratch, make sure your surface geometry is correctly created, I see a boundary surface, make sure to convert to parasolid surface using command "GEOMETRY > SURFACE > CONVERT" and mesh properly, OK?.

AXI1.png

AXI2.png

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/

Re: Contact in Axisymmetric quad element

Dear Blas,

Thanyou very much for your reply.

As you told there is an error in the nodes relation to the curve 34.

We have remeshed the model, and removed boundary surface.

 

Still this does not solve our problem.

 

Could you please let me know why. 

I have made the modification and attaching the same along with this mail.

 

Avait your reply.

 

Thank you.

 

Re: Contact in Axisymmetric quad element

[ Edited ]

Dear Sarnath,

But listen, the type of LINEAR CONTACT STATIC ANALYSIS you plan to do here is useless at all, a linear contact analysis between two regions separated with more than 10 mm is useless to solve using NX NASTRAN (SOL101), the assumption here is SMALL DISPLACEMENTS always, then nonsense to setup a linear contact problem this way, the result could be anything, useless at all, in linear contact static analysis the contacting elements should be touching each other!!.

In summary, when two surfaces are separated by a significantly initial gap (and the direction of motion is different than the surface normal), then significant errors may occur (for example, wrong location for target face stresses). If the initial gap is zero (or very small), the error may be negligible.

When contact + large displacements exist then the problem is nonlinear by geometry, and another solution sequence apart SOL101 is required to use, for instance Advanced Nonlinear (SOL601), or hopefully very soon in FEMAP v12 the MultiStepNL SOL401 that includes contact as well.

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/