Nx Nastras error using solver 101. 1

[MrJuan]

Hello, tranks for taking some minutes of your time ro read my post.

I have being working on a rin simulation following the SAE technical paper series number 2004-01-1581, they request to using hexaedrical elements on the whole assembly. I did it but I can't solve the simulation, I used two methods, "Iterative solver" and the other one, I added two pictures about the result. Any help will be great!

Sorry for my bad English, I'm a Spanish speaker.

 

[MrJuan]

http://subefotos.com/ver/?187e393a6125bc54f993705186d7bebao.png

 

[BlasMolero]

Hello!,
Your problem is easy to solve: simply go to the study name and click on "EDIT SOLVER PARAMETERS", in the nastran Command Keywords section in the MEMORY enter a value of say 1024MB, then your analysis will progress if not any error exist in the model.

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/

 

[MrJuan]

Thanks for help me, which kind of study do I have to do? Using iterative solver or the other method. I have read your answer in your blog Iberisa some days ago, but It doesn't work. I used only hexaedrical elements. To do that I split the wheel in almost 90 parts.

 

[MrJuan]

I used "contact glue-glue" to link together all the parts. Is that ok or there are other better option? Thanks again.

 

[BlasMolero]

Hello!,
Not matter you use Iterative or Direct Sparse solver, is the same related to the error memory. Of course DIRECT SPARSE solver is my preferred solver, the best accuracy at the cost of RAM memory.
GLUE surface-to-surface contact is perfect to joint parts.
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/

 

[MrJuan]

Hello again Mr Molero.

Today I was working on the simulation. I improved a little bit more the mesh quality and I didn't found the other mistakes but I got a new one. Attached you can find the picture. What can I do? I'm finishing the mesh using just tetraedrical elements.

Thanks again Mr Molero.

P.D: how important is the warning "the gap between some glue faces of some elements in gap pair"?

 

[BlasMolero]

Hello!,
Your model is not correctly constrained, you have RIGID BODY movements, then the error of SINGULAR MATRIX.
To understand the problem take a look to this post in my blog:

http://iberisa.wordpress.com/2011/0...run-terminated-due-to-excessive-pivot-ratios/

The source problem is surely related to CONTACT elements of NO PENETRATION: when using contacts you may assure that your model is correctly constrained to avoid rigid body movements: surface-to-surface contacts (as well as CGAP node-to-node explicit contact elements) conditions allow the solution to search and detect when a pair of element faces come into contact. The contact conditions prevent the faces from penetrating and allow finite sliding with optional friction effects, but allows separation between contact parts if traction loading instead compression loading exsit, ¿OK?.

You can override this fatal message by inserting “PARAM,BAILOUT,–1" in your input file: revise the animation of deformed shape to understand the error, then define constrains correctly and solve your model. DO NOT USE PARAM,BAILOUT,-1 in final runs, RESULTS could be meaningless, simply for debugging!!.

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/

 

[MrJuan]

I'm very thankful for your support. I used 6144MB yesterday in the last simulation. When I used 1024MB the same problem appeared. The error of the singular matrix doesn't appears any more but thanks to you now I know how to proceed when It happens again.

Mr Blas, which solver can I use to modelate this (I'm goint to write the sae specification):

"Since geometry and material details are critical to the accuracy of the clamping simulation, the model will be built using hex dominant three-dimensional solid elements. The stress analysis will include contact simulation and nonlinear material properties"

I'm using the solver 101 to try with "surface to surface contact" but I can't use nonlinear material properties (am I right?). Thanks for all!

 

[BlasMolero]

Hello!
The NX NASTRAN BASIC NONLINEAR solver (SOL106) do not support surface-to-surface contact, you need to use NX NASTRAN ADVANCED NONLINEAR solver (SOL601). Alternatively with SOL106 you can use 1-D CGAP 2-noded contact gap elements, but you need matching mesh between contacting parts.
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/

 

[MrJuan]

Thanks Mr Molero, Using the solver 106 sound harder compared with solver 601. I'll use that in the next days. Thanks again for your kindly help.

 

[MrJuan]

Good Morning Mr Blas, I am using the solver 601 according with your last recomendation and I got some troubles. Attached you can find a picture. What I'm doing wrong?

 

[BlasMolero]

Hello!,
The picture shows only WARNING messages, but you have TWO FATAL errors. Open the F06 file and look for FATAL, here is where you have the explanation of the error.
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/