Rigid bodies in advanced simulation 1

[Emiliano87]

Hi, I am trying to make a simple exercise of using two rigid bodies(tools) to make a plastic deformation in some kind of part. It would be a fixed rigid die and a rigid tool that pushes the steel piece to the die. I searched everywhere on how to make a body rigid in advanced simulation and I didn´t succeed. One what I found to work around this issue is to fix all degrees of freedom in the fixed die to make it rigid. But with the tool that is moving is not that simple. Am I missing something? is there a way to make some rigid body without setting a reaaaally high Elastic modulous??. Thanks for everything

 

[BlasMolero]

Hello!,
You are mixing many things: this type of problems are nonlinear, then the setup is more complex than simply linear static solution (SOL101) using surface-to-surface contact, you need to use Advanced Nonlinear Static solver (SOL601) in order to account for plasticity, large displacements & contact nonlinearities. Here you are an example of crushing an hyperelastic material between two rigid plates (

http://www.iberisa.com/soporte/femap/nolinealavanzado/brick27nodos.htm):

In NX AdvSim you need to perform two critical steps:
• Enforced Displacement constraint: in the Simulation Navigator, right-click Constraint Container→New Constraint→Enforced Displacement Constraint. You can select a face of the rigid tool, or better create a "spider-like" rigid RBE2 element and prescribe the enforced displacement contraint directly to the INDEPENDENT (master) node of the RBE2 element.
• The target contact region options: under the NX NASTRAN options of Nonlinear Contact Parameters (BCRPARA) you can set the target rigion as flexible o rigid.

For advanced nonlinear solutions (SOL 601 and 701), this parameter indicates whether a 3D contact region is a rigid surface.
• Select Flex to indicate that the region is not rigid.
• Select Rigid to indicate that the region is rigid.

For more information, see BCRPARA in the NX Nastran Quick Reference Guide and Contact conditions in the NX Nastran Advanced Nonlinear Solution—Theory and Modeling Guide.

If you select Rigid from the Type list, you will need to select the node (master grid point) that controls the motion of the rigid surface. Rigid surfaces have no flexibility apart from their rigid body motions. Internally, the software uses rigid links to connect all the nodes on the rigid target region to this master node.

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/

 

[Emiliano87]

Hi blas, Thank you for your quick answer. As I understand I have to mesh the surface with 2d meshing and set a material like if it were an elastic one. But when I define the contact and set the region as rigid and then select the master grid point the software automatically connect all the nodes of that surface to that master node, right? It would be like making spider RBE2 element from surface to the point?. So the body is made rigid in the simulation file. I was like crazy searching in the .fem file a way to set a collector like rigid. I'll give it a try and let you know the outcome. Just one thing, the master node must be a node that is in the mesh or can be a node i create lets say in the space in the center of gravity of the part? Lets say a 0D element? Sorry for my bad english my native language is spanish.

Ill take a look in those files you mention, thanks again!!

Emiliano

 

[Emiliano87]

Just another question, in the meantime I'll check the files you mention and if I find it ill post it so some other people in the same situation as me understands. In the example you mentioned I have two questions. When you specify the thickness as 0. it doesn't have problems when the solution runs?

Just finished of reading your example, really good job you have made.

Thanks again!!!

 

[BlasMolero]

Dear Emiliano,
First at all let me ask you what type of analysis you plan to run: if linear static (SOL101) or Advanced Nonlinear (SOL601), because the problem is totally different.
You have two options: to make the contact rigid (as explained above), or use regular contact between bodies and edit the Yound modules of the rigid body using a value 100x bigger, this means rigid at all.

Here you are an example of metal forming simulation using Advanced Ninlinear module (SOL601), here the matrix stabilization parameter MSTAB=1 in NXSTRAT is used in order to stabilize static problems with rigid body modes, if not will appear problems of singular stiffness matrix error.

YouTube Video

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/