×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Help needed for NX nastran
2

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.

RE: Help needed for NX nastran

Your model is not properly constrained, review your boundary conditions

Seif Eddine Naffoussi, Stress Engineer
www.Innovamech.com
33650 Martillac û France

RE: Help needed for NX nastran

(OP)
yes sir I know but its not working out.The problem is with sphere I think so because if I don't include sphere it is working but adding sphere doesn't work.

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

May be you should create a spherical coordinate system and then fix some Degree of Freedom for some nodes just to avoid the rigid body motion.

Seif Eddine Naffoussi, Stress Engineer
www.Innovamech.com
33650 Martillac û France

RE: Help needed for NX nastran

(OP)
kk sir I will try it now.

RE: Help needed for NX nastran

Hello!,
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

(OP)
Sir I have given constraints but I cant figure out what mistake I am making.Actually I am new to NX.

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

Hello!,
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

(OP)
Sir cant get cant get you...

"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

(OP)
Sir I am getting error "Result is in wrong format".

Please help me

RE: Help needed for NX nastran

(OP)
can we select a point or a node for giving constraints as when I select, whole surface gets selected.

A point or a node for giving constraint ?

RE: Help needed for NX nastran

(OP)
@BlasMolero sir can you tell me what constraint you gave to the sphere?

RE: Help needed for NX nastran

Hello!,
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

(OP)
Thank you for the reply sir.I will try it to constrain the three nodes as you told and also try it with SOL103.Thank you

RE: Help needed for NX nastran

(OP)
Sir its not working for me.Means its showing deformation but its not squeezing between the plates....

I need to do in SOL101 or 601.

RE: Help needed for NX nastran

Hello!,
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

(OP)
@BlasMolero,

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

Hi Harshitbhatt,

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

(OP)
@Tuw thanx for the reply sir.

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

Hello Harshitbhatt,


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

(OP)
@Tuw thanx for the reply sir.The moving plate is actually a ring which will rotate and this is how its moving, not horizontally.I have taken just a part of the whole ring. All this parts are 360 deg.I have taken just 1 deg.

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

Hi Harshitbhatt,

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

(OP)
@Tuw thank you for the reply sir.Sir I saw the file you attached.Thank you for your valuable time.Actually I need to find out the deformation of O ring[Cylinder] and while it deforms what deformation we get in another two. I have attached my simulation.If you can see to it.

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

Hi Harshitbhatt,

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

(OP)
@Tuw Thanx for this reply sir.Helped lot.I will do it as you said.....

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

Hi Harshitbhatt,

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

(OP)
@Tuw thank you sir.Actually when I click on help in my NX 9 its not opening.Its showing some cannot connect to html file.My version is student version.

RE: Help needed for NX nastran

(OP)
@Tuw Sir I did the same but not working .......

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.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources