Axi-symmetric modeling UG/NX

[Serbet]

Hi,

I am trying to model a compound cylinder in NX 6 using Nastran. The model would be an Axi-symmetric problem with the inner and outer cylinders modeled in perfect contact. The problem is that I do not have a clear understanding of how model the contact. Should I use 'Contact mesh'? If so, how do I set the contact elements. Any help would be appreciated.

Thanks,
S.

 

[BlasMolero]

Dear Serbet,
Axisymmetric analysis lets you solve an FE model that is defined for only a section cut on one side of the axis of an axisymmetric part. Axisymmetry occurs when the geometry is a solid of revolution with a constant cross section, and loads and constraints are only radial and axial. This greatly reduces the degrees of freedom (DOF) and hence also significantly reduces solution time. Axisymmetric analysis requires that the center of rotation and radial axis of the axisymmetric model be properly aligned to the absolute coordinate system. For the NX Nastran solver:

• The axisymmetric axis is absolute Z
• The axisymmetric plane is absolute XZ for positive X
• This means the model must lie in the +X half of the XZ plane.

Said that if you solve a model as axisymmtric forgot at all to use any geometry-based contact resource like surface-to-surface or GLUE surface-to-surface, these are for general contact with Shell or solid models. The only valid contact resource available is to model "explicitely" the contact using 1-D contact CGAP node-to-node elements.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[Serbet]

Dear BlasMolero,

Thanks for the quick response. I have been trying to model the contact using 'Contact mesh' which I believe defines 1-D elements to model contact. The thing is that I do not fully understand their definition. Do I have to create a number of 1-D elements equal to the number of nodes at each contact edge? And, does these elements are defined as simple springs or do they have a more complicated definition?

Thanks,
S.

 

[BlasMolero]

Dear Serbet,
In fact, is not well explained, but is very simply if you know what is a CGAP element from NX NASTRAN: you need to use Edge Contact Mesh to create point-to-point contact between two edges or a portion of two edges defined by limiting points. You can only use Contact Mesh to create a contact mesh on between edges on your model's geometry. This means, for example, that you cannot use Contact Mesh to create a contact mesh between elements you created manually using commands on the Element Operations toolbar.

You need to define EQUAL number of nodes to every contact edge. Also, once you create a contact mesh, you can modify the contact mesh Z direction if necessary. The Z direction should be normal to the contact face and contact element using EDIT MESH ASSOCIATED DATA. Also you need to edit the CGAP property (PGAP card) to enter both THE AXIAL STIFFNESS FOR CLOSED CGAP ELEMENT (use a value like 1e6) and THE INITIAL GAP OPENING.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/