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
- CAE Simulation - NX Nastran Forum
- simulate an ensemble

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

01-26-2014 01:28 AM

HI,

I loaded a ".asm" ensemble of 2 solids with diferent materials properties in NX 8.5 and made a NX NASTRAN 106 nonlinear simulation, but the program doesn´t find results.

Is there a special tip for restrictions or forces or meshes to solve a nonlinear analisys of an ensemble with diferent materials properties?

I need two simulate simple flexion with two solids one over the other each of them with different materials properties. How can I do this?

Thanks,

Daniel Hoyos

Escuela de Ingenieria, university.

3 REPLIES

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

01-26-2014 06:06 AM

Dear Daniel,

Take a look to the *.F06 file located in the same directory of the *.PRT or *.SIM file, open with a text editor and look for the word FATAL, there you will have the description of the NX NASTRAN error. As you are talking about Assemblies + NonLinear analysis with BASIC NX NASTRAN (SOL106), then I guess the error will be related with any singular matrix dure to rigid body motion (take a look to my blog here: http://iberisa.wordpress.com/2011/02/20/mensaje-de-error-de-nx-nastran-run-terminated-due-to-excessi...).

In fact, you need to constraint properly components in the assembly in order to avoid rigid body movements that will cause singular matrix and then FATAL error in the nx nastran solver.

Also please note that BASIC Nonlinear NX NASTRAN solver do not support surface-to-surface contact (like in linear static SOL101), so in order to define the "contact interaction" between bodies in the assembly you need to use either explicit 1-D CGAP node-to-node elements or "slideline" contact feature.

The 1-D **CGAP** element is intended to model surfaces which may come into contact. When positive pressure exists, the gap can carry any transverse shear load which is less than the coefficient of friction times the normal load. The CGAP element connects two grid points which may be initially coincident. * There is no geometric nonlinear behavior, which implies that the orientation of the contact plane does not change during deflection*. Then, if you are dealing with "large displacements" and "large deformation" nonlinear problem then better use the NX Nastran Advanced Nonlinear module (SOL601) that fully support contact surface-to-surface as well as other nonlinearities.

The other contact option for SOL106 is the "point-to-line" **slideline contact**: is capable of modeling nonlinear contact geometry and inelastic material behavior including large deformation. Slideline contact is useful for two dimensional geometries, for example plane stress, plane strain and axisymmetric. They can also be used for three dimensional geometries provided the contact between the two bodies can be defined in terms of parallel planes called the slideline planes. The sliding and separation of the two bodies is restricted to the slideline planes. The bodies can have large relative motions within the slideline plane. However, relative motions outside the slideline planes are ignored; therefore, they must be small compared to a typical slideline element.

In summary, to be practicall, if you are working with NX AdvSim + NX Nastran as your solver and not access to Advanced Nonlinear Solver (SOL601), then the only resource is to use CGAP elements: go to FEM environment and use command from menu "* Insert > Mesh > Surface Contact Mesh*" that will lets you create and define contact elements between two selected faces of a solid or between different components. This way you are defining contact elements as "

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

01-27-2014 12:02 PM

Thanks Blas,

I have another question. If I want to analyse a 105 linear buckling solution with the same criteria of the ensemble, must I do the same procedure you suggested for the 106 non linear analysis?

Thanks,

Daniel Hoyos

Escuela de Ingenieria, university

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

01-27-2014 12:50 PM

Dear Daniel,

Yes, in fact, Contact conditions (surface-to-surface contact) as well as GLUE surface-to-surface can be included in a Linear Buckling solution (SOL 105) since NX AdvSim 8.5 with NX NASTRAN V8.5, although there are important considerations:

- The inputs for a linear buckling solution with contact conditions require a subcase for the linear statics subcase and the buckling solution.
- In addition, the linear statics subcase must include the BCSET case control command. If the linear statics subcase is the first subcase, then a STATSUB bulk entry is not needed. If it is not the first subcase, a STATSUB bulk entry is needed in the buckling subcase to reference the linear statics subcase ID.

All of the above is "transparent" for the NX AdvSim user, simply define contact surface-to-surface and you are done!.

Best regards,

Blas.

PD

If you find my post helpful, and it answers your question, please mark it as an "Accepted Solution" -- thanks!.

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