Help needed for NX nastran
Help needed for NX nastran
(OP)
I need help in doing simulation for finding deformation of a model but I am getting the following error:-
"SYSTEM FATAL MESSAGE 3000 (SITDELC)
ITERATIVE SOLUTION FAILED DUE TO FAILURE OF PRECONDITIONER TO FACTOR.
THIS ERROR CAN RESULT IF THE STRUCTURE IS NOT RESTRAINED SUFFICIENTLY TO PREVENT
RIGID BODY MOTION OR IF INTERNAL MECHANISMS EXIST."
Please help me out.
I have attached my file for the reference.
"SYSTEM FATAL MESSAGE 3000 (SITDELC)
ITERATIVE SOLUTION FAILED DUE TO FAILURE OF PRECONDITIONER TO FACTOR.
THIS ERROR CAN RESULT IF THE STRUCTURE IS NOT RESTRAINED SUFFICIENTLY TO PREVENT
RIGID BODY MOTION OR IF INTERNAL MECHANISMS EXIST."
Please help me out.
I have attached my file for the reference.





RE: Help needed for NX nastran
Seif Eddine Naffoussi, Stress Engineer
www.Innovamech.com
33650 Martillac û France
RE: Help needed for NX nastran
When I modeled the geometry it was showing fully constrained and when doing simulation its giving the constraint error.
RE: Help needed for NX nastran
Seif Eddine Naffoussi, Stress Engineer
www.Innovamech.com
33650 Martillac û France
RE: Help needed for NX nastran
RE: Help needed for NX nastran
Your model is not properly constrained as Seif explained, the sphere is free to "fly", if you run a modal/eigenvalue analysis using NX NASTRAN (SOL103) you will see the six rigid body motions in the sphere as six modes of value 0.0 HZ(the SIX DOF), the bofy is perfectly free to move in the space, and this is wrong in FEA: to get a valid solution you need to constrain your structure.
Best regards,
Blas.
~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director
IBERISA
48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog de FEMAP & NX Nastran: http://iberisa.wordpress.com/
RE: Help needed for NX nastran
The screen shot you posted, I think may be I am wrong, you must have given fixed constraints to both the plates but I need to give pressure on the plates and also the sphere and see the deformation [Both plates and sphere].
Can you please give me the files you have run if possible.And thank you for your comment.
RE: Help needed for NX nastran
Well, is your model, yourself you can click in the FIXED constrain and you can see that the sphere is free, the model is not properly constrained, then the error ..
Best regards,
Blas.
~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director
IBERISA
48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog de FEMAP & NX Nastran: http://iberisa.wordpress.com/
RE: Help needed for NX nastran
"Well, is your model, yourself you can click in the FIXED constrain and you can see that the sphere is free, the model is not properly constrained, then the error .." srry
RE: Help needed for NX nastran
Please help me
RE: Help needed for NX nastran
A point or a node for giving constraint ?
RE: Help needed for NX nastran
RE: Help needed for NX nastran
I didn´t gave any constraint to the sphere, I arrived to a solution because I ran a modal eingenvalue analysis (SOL103) where a free-free analysis could be performed: the analysis shows the rigid body motions that exist in a FE model and cause a singular matrix error in a Linear Static Analysis (SOL101). Please take a look here: https://iberisa.wordpress.com/2011/02/20/mensaje-d...
In summary, if you want to arrive to a valid solution running a Linear Static Analysis (SOL101) you will have to constraint at least three (3) nodes of the sphere (not co-linear) in order to remove the rigid body motions in the sphere.
Best regards,
Blas.
~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director
IBERISA
48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog de FEMAP & NX Nastran: http://iberisa.wordpress.com/
RE: Help needed for NX nastran
RE: Help needed for NX nastran
I need to do in SOL101 or 601.
RE: Help needed for NX nastran
If you want to simulate "the ball squeezing between the plates" then you need to define surface-to-surface contact between the sphere faces & plate faces. Because you have a gap distance between the sphere faces and the plate faces, then the problem could not be solved as a linear contact problem using NX NASTRAN (SOL101) because you have large displacements, then the problem is fully nonlinear for the geometry: you will need to use Advanced NonLinear Solver (SOL601). A linear contact solution here is useless, simply colors ...
Best regards,
Blas.
~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director
IBERISA
48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog de FEMAP & NX Nastran: http://iberisa.wordpress.com/
RE: Help needed for NX nastran
Yes sir I did the same.Surface to surface contact and SOL601.But its not squeezing between the plates.....
Cant understand what mistake I am making
RE: Help needed for NX nastran
About constraint, you did not apply any constraint at the sphere, even though you applied fixed constraint at the other 2 components. The solver will fail definitely in Sol101 because the ball is not fixed at all.
I don't understand what is your analysis objective is, but my suggestion is probably you can try to create a symmetry line to the ball, then apply symmetry constraint at the ball (provided you need to understand what and how to define a symmetry condition constraint using the user-defined constraint).
I noted that you would like to define constraint at "node" instead of "polygon surface". Yes it can be done, simply drop down from the No Selection Filter Drop Down List in the Selection Bar, and choose the Entity "Node" will do.
That's all about constraint. Next, even with constraint, the ball still cannot reach equilibrium without the support from its neighboring components. Therefore, you need to define contacts, like what Blas mentioned. To further enhance the contact between the sphere and its neighboring components, you can try to define a gravity load, which the direction of the gravity load helps to promote the contact definition (not the opposite direction with defy contact).
In my opinion, you can still try Sol101. If you need more help, please provide detail explanation on what your analysis objective is.
Regards,
Tuw
RE: Help needed for NX nastran
I did all what you said.Here is short description what I need.
My problem has two plates,one moving and one is fixed.There is a plastic cylinder between the two and presuure is acting on both the sides of cylinder and also on the two plates.
When I am running the simulation I am not getting the exact result which I should get[Deformation of the cylinder].The cylinder should squeeze in between two plates. My project detail [2D].
Here in 3D
I have uploaded my simulation file.If you can please see to it.
RE: Help needed for NX nastran
1. The Moving Plate is applied with a Fixed Constraint. So you want to move the plate, or you want to fix the plate??
2. The left side of the Moving Plate is 10bar, the right side is 20bar, so the Moving Plate should be moving to left side (due to pressure difference) or right side (as indicated by you to make contact with the cylinder)?
RE: Help needed for NX nastran
I have fixed the CG of moving plate as I need to find deformation of whole plate.The cylinder should deform between the two plates.The upper surface of cylinder has 20 bar pressure and lower surface has 1 bar pressure.So due to this it should go towards the left side of two plates.The cylinder is a O-ring. This is actually a DRY GAS SEAL.
RE: Help needed for NX nastran
Please find attached file for your reference.
For your information, your loading condition is pressure, which is quite challenging because pressure or force load would induce inertia effect. In order to ignore the inertia effect, I change the pressure loading to enforced displacement, which is better in convergence. Again, this goes back to your analysis objective, what is your analysis purpose? will this act against your purpose..
All in all, you have a lot to study...
RE: Help needed for NX nastran
When you will see the result,you will see that when O ring is getting in between the two,the edge of upper plate gets deform.I was looking for that but still the O ring should squeeze in between the two[change its shape for like circle to oval or something].This is not happening.
Thanx for the reply sir.......
RE: Help needed for NX nastran
There are many reason/factor to view deformation. Some point you should take note.
1. Your analysis is considered as high complexity or nonlinearities. Therefore, when you build your simulation model, please do it by adding complexity gradually and slowly. The way you do contact definition is not recommended, because you are trying to dump everything/ every surface into 1 definition. Remember, split the definition into several simpler definition, 1 surface versus another 1 surface. This is the way of professionalism.
2. When you are working with Sol601106, that means your are taking into consideration of boundary nonlinearity or time. If you want to see deformation, define a time. We don't expect the deformation can be achieved within 1 single loop of iteration, do we?
3. Furthermore, if you insist of using pressure or force loading condition, I think the more suitable solution would be Sol601129, which take into consideration of inertia effect. Please take note that for this solution, you will need to have very fine time step (i.e. 0.0001sec per step or smaller). You might have challenge to get the right time step to achieve convergence.
4. Did you define a proper o -ring material using the correct material model, for example hyperelastic material model? Did you have the material data sufficient, for example the stress strain curve?
Please don't expect to get a quick solution here. A successful and meaningful simulation is tonne of hardwork and patience.
Regards,
Tuw
RE: Help needed for NX nastran
Thank you for your reply.And what should I do in my simulation to get better result.First of all is it correct?
The file I uploaded.
RE: Help needed for NX nastran
Good question. This address lack of confidence. Always beginning your simulation with a simple one. For example, you can just do a simple compression simulation between 2 components, not necessary to follow the actual geometry. It can be a cuboid and another sphere. Check the deformation whether as expected. If not, there is no meaning to add more complexity, but to focus on this study. Then, once you achieved this, add more complexity, 1 by 1. Do 1 study at a time. This is the way to gain confidence. The truth is your work is not professional.
Some study you may consider:
1. Use enforced displacement first, before proceed to use pressure loading because it is more difficult to converge.
2. Use user-defined constraint. Learn about DOF (degree of freedom).
3. Use Sol101 first before using more complex solution. Understand limits of Sol101 (linear static).
4. Learn about meshing, geometry idealization and mesh quality.
5. Learn about to constraint your model in cylindrical coordinate system .
6. Get the material specification of the o ring. Study hyperelastic material model.
7. Learn time step setting up.
8. Learn strategy parameters for Advanced solution Sol601106 and Sol601129.
Look up NX Documentation for explanation.
RE: Help needed for NX nastran
RE: Help needed for NX nastran
http://www.eng-tips.com/viewthread.cfm?qid=354003
RE: Help needed for NX nastran
No I will try IIS.I didnt do that.
Maybe its student version so it may not work but I will try IIS.
Thank you sir.