NX: problem with results

[ArthurFormiga]

Hello,

I'm having some problem to get the results of a linear static analisis, i've applied the loads, the constraints, and the surface-to-surface contacts, in the .f06 file, i found the error: RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIO, I set the bailout to -1, so I could see the error, and the problem was in one bolt, the maximun displacement was 75mm on it. I just can't find the reason of that.

Thank you,
Arthur Lisboa

 

[Walterke]

post a picture of the result

NX 7.5.5.4 with Teamcenter 8 on win7 64
Intel Xeon @3.2GHz
8GB RAM
Nvidia Quadro 2000

 

[ArthurFormiga]

http://imageshack.us/photo/my-images/835/stressj.jpg/

This is the STRESS result

http://imageshack.us/photo/my-images/259/displacement.jpg/

This is the DISPLACEMENT result

 

[BlasMolero]

Dear Arthur,
Is evident you have a problem of rigid body movement, please note that defining surface-to-surface contact do not assure the properly constrain of a component, it simply avoid penetration between touching faces, but the rest of movements are free unless you prescribe properly global constraints or local joints, then is up to you to assure that the component DOF are properly constrained.

You can use GLUE surface-to-surface where not relative movement between components exist.

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/

 

[ArthurFormiga]

Dear Blas,

Thank you for your help, I added some new constraints to prevent rigid body movements, but I got the same error. So, I activated AUTOSPC, in PARAM, and everything seems to work properly now. My question is, when i activated AUTOSPC, what I'm really doing? It's only a way to prevent elements' movements?
Could you tell me which version of NX do you work with?

Best regards,
Arthur.

 

[BlasMolero]

Dear Arthur,
In the modern versions of NX NASTRAN (I run 8.1) the command "PARAM,AUTOSPC,YES" is activated by default (in all SOLs, except 106, 129, 153, and 159) NX Nastran automatically removes degrees of freedom that are either unconnected or very weakly coupled to the finite element model, but AUTOSPC do not remove singularities when your model is not properly constrained, OK?.

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/

 

[ArthurFormiga]

Dear Blas,

I'm starting to work with NX now, this is my first simulation, so I have some other doubts, if you don't mind.

1- I'm trying to proper constraint every rigid body, in the bolts and washers, I've putted a pinned constrain, and fixed constraint in axles Z and X, but when I do that (fixing the bolts' movements in axle X), I'm 'canceling' every force that acts along X?

2- If I'm performing a linear static analysis, it means that I only have forces along one axle?


Best regards,
Arthur Lisboa

 

[BlasMolero]

Dear Arthur,
If you have bolts in your FE model you can't prescribe GLOBAL constraints, but localy define the coupling using RBE2/RBE3 rigid elements or MPC multi-point constraints. Better ask to receive a training course from your VAR provider, this is extremely important to have a clear knowledge of the basics & fundamentals of NX Advanced Simulation, OK?.
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/

 

[ArthurFormiga]

Dear Blas,

Thank you.


Best regards,
Arthur Lisboa

 

[BlasMolero]

Dear Arthur,
Well, I understand that you are student, but not excuses, the use of engineering tools of Finite Element Analysis requires competence, anybody can use a CAD system to create a solid model of an engine, not need to be engineer, but FEA tools are powerful tools that requires experience & knowledge, and it is only a question of time ... years. Here you are some comments to your model:

1.- All the bolts (shanks, nut & washer) of your 3-D CAD model are meshed with solid tetrahedral elements, and used a surface-to-surface contact of NO PENETRATION between bolts & parts. Well, you may understand that surface-tu-surface contact avoid the penetration of wahser in nut, or washer & body, etc.., but do not prevent the separation between parts, then a singular matrix error will appear for sure!!. The problem is the approach used to model bolts AS SOLIDS: not, a better approach to model bolts is to use the Bolt Connection command. The Bolt Connection command automatically creates an element that represents the shank of the bolt and a pair of spider elements (RBE2/RBE3 NX Nastran rigid elements) that connect the ends of the element to the surrounding mesh. Please note:

• You can use the Circular Imprint command to define the surfaces around the bolt hole that are under the heads of the bolt and nut. By imprinting these surfaces, the legs of the spider elements that are created using the Bolt Connection command are automatically connected to all the nodes within the imprinted surfaces.

• With NX Nastran solver the elements representing the bolts are CBEAM or CBAR, then you can use the Bolt Pre-Load command for direct entry of bolt preload forces.

2.- You have prescribed EXTERNAL boundary conditions to the bolt solid faces of type "pinned". Not correct at all, you can´t prescribe external constraints to bolts, this should be done using "INTERNAL" 1-D connections that define relations of multi-point constraints (MPC) between components DOF. Well, these are the RBE2/RBE3 rigid elements available in NX NASTRAN, more easy & powerful, frequently used as spider elements: An R-type element is an element that imposes fixed constraints between components of motion at the grid points or scalar points to which they are connected. Thus, an R-type element is mathematically equivalent to one or more multipoint constraint equations. Each constraint equation expresses one dependent degree of freedom as a linear function of the independent degrees of freedom

in the following picture you have an example of using bolts in an assembly where an spider element is defined as a single core node that is connected to multiple leg nodes with rigid or constraint elements.

Hope it helps.

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/