NX Nastran Contact analysis

[drkcyde]

Hello all,

I have been using UG for years but I am new to the FEA nastran analysis. I have been trying to apply a contact between two surfaces. I set up everything and run the solution but I am getting an error message that say that my surface contact is conflicting with boundary condition/loads.

Basically, I am trying a simplified model where I just have two blocks mated together. One block has a fixed surface and the other block has an applied pressure to a surface. The surface where they interact I have applied a surface contact condition where I let UG automatically pick my surfaces.

Does anyone have exerience in contact analysis with UG NX Nastran.
I am also running advance non-linear 601

Thank you for your help and reading my post
-Andrew

 

[GBor]

Andrew,

I'm not an NX user, but contact analysis is pretty much the same throughout most of the packages in terms of the problems they may cause, so a few questions:

How far apart are the surfaces that are supposed to contact?

What is your time step?

How much mass exists in the moving block?

What pressure do you have on the block?

One of the typical problems is time step is too large, so the moving contact surface drives through the mating surface too far for the contact algorithm to engage. Sometimes it is contact stiffness is too large or too small. Plethora of other settings...

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.
Lower Alabama SolidWorks Users Group
Magnitude The Finite Element Analysis Magazine for the Engineering Community

 

[drkcyde]

Garland,

Thank you for you response. To answer a couple of questions, the blocks are just about 1mm apart and they are 2"x2"x2" in size, so the mass is quite low.

What I have noticed is that there is problem with the meshing. Once I run the simulation, there is an error that say that the nodal corners of the 3D elements are not connecting to each other. I seem to be having this issue with the advance non-linear solution of nastran.

Just as a test, I decided to just mesh a single block with a linear static solution and it worked, so I know something is happening with the advance non-linear solution in nastran.

I also seem to be having an error which refers to something known as ISHELL?!?! Of course, the nastran help is tripe, and it doesn't shed any light on this issue.

Thanks again for your help,

-Andrew

 

[GBor]

Again, not knowing NX Nastran (anyone feel free to jump in and bail me out, here), it is difficult to diagnose, but I would suggest reducing the problem to 2-D and seeing if you can run it as a plane stress or plane strain problem. Line the nodes up as best as possible and just use gravity as the load instead of a pressure. Pin the bottom edge of the lower block and let the top block fall under the effects of gravity. Based on the mass, you can hand calculate how far is would fall during a certain time step. Separate the blocks by that amount, and reduce the time step by AT LEAST 1/4, so that there will be 4 time steps before contact is made...this just lets you see what happens. You can even pin the sides of the falling block so that it can only travel vertically.

It sounds like, with only a 1mm seaparation, the moving block is going too far through the stationary block to notice the contact.

One last comment: you state a separation of 1 mm, but a size in inches. Realize that the processor is either interpreting the separation as 1/25" or the block size as 2x2x2 mm and make certain that the units of your material property data, gravity, pressure, etc. are all consistent and correct.

 

[Ronald62]

Andrew,

I've been using NX + contacts a lot. NX has very good contact algorithms. SOL101 has the algorithm from Ideas and SOL601 has the algorithm from Adina. Both of those work well.

Have you built the model with shell or solid elements?

Have you connected those parts to each other using springs, rods etc.? It's important to fix parts together because the contact is not exist in the beginning.

Have you tried to solve the problem using linear contact? I mean using SOL101.


The "Error message manager" of NX is very poor in my opinion so it may be difficult to find out the reason. Good luck!

 

[drkcyde]

Thank you again Garland for responding, and thank you Ronald for your response. I think I will start from the beginning, and hopefully this will answer everyone's questions.

My project I am working on is an interaction between two faces for a coolant delivery system for our CNC grinder. Modeling the part was simple, but the FEA was new to me, so I thought that I would start with doing an analysis with just two arbitrary blocks to get a feel for the nastran package in UG.

What I have done is simply modeled two blocks that are the same size and mated them together with a 1mm gap (arbitrarily picked)

I then initiated the advanced simulation package and defined one block as brass and one as steel (just to have one softer than the other) I then did the following steps to prepare for the analysis:

solver: nx nastran
analysis type: structural
solution type: advnl 601,106

physical properties: psolid
integration network: bubble
stressoutput location: grid
integration scheme: reduced

mesh collector: 3d
collector type: solid

3d swept mesh

contraints: one side of brass fixed
loads ressure load on opposite side of steel block

simulation object type: advanced non-linear contact
->I left everything else in that window as default values

So to answer one question, I am using solid elements. For my nozzle, I am using a 2D shell then extruding/revolving the elements to get a uniform shape. To answer another question, I am using a face to face contact to define the contact between the two opposing faces.

I have tried to solve using SOL101, but nastran gave an iteration error, that is when I switched to ADVNL601.

I should quickly mention that I am using 50mm cubes with 25mm solid brick elements, so 4 elements per block.

After I set up everything and solve, the solver runs to completion, but when I check the solution, I get the following errors:

NASTRAN Msg: ***WARNING: THE FOLLOWING LIST SHOWS UNSUPPORTED FIELDS FOR CERTAIN
BULK DATA
ENTRIES PROCESSED IN THIS INPUT FILE. YOUR MODEL MAY BE
AFFECTED
NASTRAN Msg: ***WARNING: No element connection for node 1 directions 4, 5, 6
***WARNING: Similar warning suppressed for 44 other nodes.
NASTRAN Msg: ***WARNING: Nodal degrees of freedom without element
connection have been fixed for data input file.
NASTRAN Msg: *** SYSTEM FATAL MESSAGE 7355 (ISHELL)
ISHELL PROCESSING FAILED.
NASTRAN Msg: ^^^ USER FATAL MESSAGE
^^^ ERROR IN ADVANCED NONLINEAR MODULE -1

Total messages: 3 WARNINGs and 2 FATALs

One thing that I noticed is that the only nodes that are considered connected are the nodes where the constraint is applied.

Thank you everybody for reading this, and I know your eyes likely hurt after it (I know my fingers do )

-Andrew

 

[Ronald62]

I recommemd that you should try to solve this problem using linear static solver (SOL101) without any contacts. Or make an eigenvalue analysis.

If the analysis works fine, then try to solve this nonlinear with contacts.

SOL106 doesn't have surface contact capability so you can forget it. It has only gap contacts.

 

[drkcyde]

Hi Ronald,

I went back and tried using the linear solver, but instead of using quad elements, I just used the tetrahedral, and I also used two different shaped objects (for fun). I used a contact mesh instead of applied and surface to surface contact and I got some results!!!!!

Now to try to get this working with my nozzle head ;-)

Thanks for your help
-Andrew

 

[Ronald62]

Hi Andrew,

Did you use previously shell elements? Are you sure you properly defined offset values?
The contact doesn't work if the offset values are wrong. You have to also carefully define the maximum search distace of the contact. If that value is smaller than the distance between the contact surfaces, the slave surface doesn't find the master suface so the contact is not exist.

Those are important things when using shell elements.

Ronald