Is there any Femap documentation/Tutorial on how to perform a deformable-rigid body contact analysis?
To start with
I am trying to simulate a L-bracket, whose base flange is supported by a rigid surface underneath and the upstanding flange of the L-bracket sees an eccentric compression load. Mainly interested in the deformation pattern of the base flange.
I tried but got 101 fatal errors. I had meshed the deformable surface using plate elements with a material definition of E=1e11 psi and nu = 0.3. The thickness of the rigid surface was 0.1" and I had defined rigid connection property.
Looking back, the other step I had missed was fixing the rigid body surface. I am assuming that applying a fixed SPC would work?
Anyways, I would appreciate if there a Femap tutorial on deformable-rigid body contact.
Thx in advance,
What solution are you using - Advanced Nonlinear?
There's an example of using rigid body contact here:
Thanks for the workshop link Chip.
Since I am not really interested in stresses currently, I will just try a linear static/buckling initially. Want to get the model run without any issues to start with
Mostly interested in deformation pattern at the moment. I will post here if I have further issues. Appreciate the help from Femap community.
Was going through Femap Commands manual and noticed this at 184.108.40.206 Type of Segment:
"Note: A Connection Region used for Linear Static Analysis for NX Nastran has the same definition as
Advanced Nonlinear except Type cannot be set to Rigid and the Ref Node is not available. For 3-D con-
tact in Advanced Nonlinear (SOL 601 and 701), the “Rigid” Type can only be used for a target Connec-
tion Region when the Contact Type is set to Rigid Target in the Connection Property. Finally, For 2-D
Contact in SOL 601, the Rigid option can also only be used on “target” regions and allows you to use
Ref Node to specify a rigid reference node.
Ref Node (Rigid Body Reference Node)
The Ref Node is used to apply constraints and motions to the rigid segment. Constraints and motions (displacements, velocities, etc.) assigned to the reference node will be assigned to the rigid segment.
For NX Nastran, in both 2-D and 3-D contact the Ref Node will written to the “MGP” field of a BCRPARA entry
along with a corresponding RIGID in the “TYPE” field."
I have gone through the pdf of the workshop provided by Chip and haven't gone through the Femap file, but I am getting confused with the Ref Node. Should the Ref Node be at the center always. If I have applied BC to curves (or faces) of the rigid geometry, per the literature above, these constraints won't be applied to rigid contact body unless them constraints are applied through Ref Node, correct?
Lastly, if the rigid bodies need to be meshed, I think a material and property card definition are needed as well?
The Reference Node does not need to be at the center of the Rigid Connection Region. And, you should only apply a constraint on the Rigid Connection Region at the Reference Node, not to any other nodes on the Rigid Region.
Yes, you must apply a material and a property to the mesh in the Rigid Connection Region. These will be ignored by Advanced Nonlinear as the Rigid Region internally used the element faces as the rigid contact surfaces.
You should refer to the Advanced Nonlinear Theory and Modeling Guide under the Help > NX Nastran menu in Femap.
I have one more question on the above. I was able to run successfully a rigid contact with rigid geometry having 3D elements. Is not possible to have a rigid CQUAD4 definition in SOL601. I am getting the following error:
"*** Reading Nastran data ...
***WARNING: THE FOLLOWING LIST SHOWS UNSUPPORTED FIELDS FOR CERTAIN BULK DATA
ENTRIES PROCESSED IN THIS INPUT FILE. YOUR MODEL MAY BE AFFECTED
IF VALUES ARE ENTERED IN THESE UNSUPPORTED FIELDS.
* ENTRY : UNSUPPORTED FIELDS / RESTRICTIONS *
* PSHELL : MID2, 12I/T**3, MID3, TS/T, NSM, Z1, Z2, MID4 *
* : *
***ALERT: Node 2192 cannot be a rigidlink slave
since it has one of its displacement degrees of freedom fixed.
*** Model errors exist - file tmpadvnlin.dat has not been created.
Please resolve conditions indicated by ERROR or ALERT
messages given above.
*** Allocating 12748 MB of memory ...
*** FATAL ERROR: PROCESSING OF NASTRAN DATA FOR SOL 601 FAILED.
*** ADVANCED NONLINEAR EXIT CODE 0 ***
*** ISHELL PROGRAM 'NXNA' COMPLETED ***
^^^ USER FATAL MESSAGE
^^^ ERROR IN ADVANCED NONLINEAR MODULE 0
^^^SOL601 FAILED "
So far, I have not come across in NX ANL Manual, where a limitation of using 2D elements as rigid target is published, excpet when the contact algo is set to "Rigid Target". I believe that algo only works with 3D elements.
Rigid Contact is supported for 2D elements and they are used in the example that I posted on this forum in the Knowledge Base. I recommend you add a "free" node without a connection to any element and assign that as the the Reference Node for the rigid connection region. Constraints, and enforced motion should be assigned to that node.
Also, check your material and property used for the rigid connection region. The only material attributes needed are E and G or nu.
THanks for reply.
I did go through the workshop...somehow I was unable to understand it in its entirety.
I wanted to post pictures of my model setup along with definition of key terms and make sure I've not missed anything important.
All units are imperial. And in the contact connectors definition, master surface is assigned to rigid body.
THere is a compressive load and moment acting on the upstanding leg of the L-fitting. Also a fixed DOF BC is applied to a center node of the base bolt hole via RBE2 connection. The rigid surface is supposed to simulate abutting surface. Also the rigid surface has a fixed BC via Node 2192.
I would appreciate if could let me know if any mistakes in the above definition.
You need to specify a G or nu value for your Rigid material, otherwise, NX Nastran will give you a fatal error.
Also, it looks like the rigid contact surface is embedded into the flexible body. When defining a rigid connection region, the thickness of the element is ignored unless you specify an offset as part of the rigid connection region.
You can either post your model here or directly email it to me as a .zip file to firstname.lastname@example.org