NX Nastran: Pressure Vessel Analysis

[Lunder]

Hello,

I am currently learning NX Nastran and I am trying to perform an analysis of a pressure vessel I have designed. I have been using SOL 106 - Global Constraints and have got some results, but it took about 6 hours to run. So my question is, is SOL 106 the best alternative? How would you set up the analysis?

I used fixed constraints on the pressure vessels support legs, internal pressure 1.1 MPa, and surface-to-surface gluing between the main body and the two end caps. Part file attached.

Thanks!

 

[BlasMolero]

Hello!,
The important file is the *.modfem FEMAP model, more than the *.prt geometry file, then we will see the meshing aproach used to mesh the vessel.
The Nonlinear solver (SOL106) is always the exact solution (real life is always dynamic transient & nonlinear!!), of course, but it could have an important cost in both solution time & hardware resources, so I strongly suggest to run FIRST always a linear static (SOL101), evaluate results of both displacements & stress, and judge if a nonlinear analysis is required. If you have displacements results of the order of the pressure vessel thickness, then please run a nonlinear analysis, because linear static analysis do not account for stiffening effects due to inplane loadings: the way that tensile mebrane stress increases the bending stiffness is computed by nonlinear analysis only.

Here you are a simply vessel example solved with FEMAP & NX NASTRAN as linear & nonlinear (considering only large displacements effects geometric nonlinearity), comparing both solutions of displacement results vs. load you will realize the level of nonlinearity of the problem:

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/

 

[Lunder]

Thank you, BlasMolero, for a informative post!

I have been trying to run SOL101 for quite some time, but it will not solve. I am setting everything up just as I have done in SOL106, and I get this fatal message in the .f06 file:

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.

I use surface-to-surface gluing and fixed constraints, so I dont know what more to constrain. Any ideas?

 

[BlasMolero]

Dear Lunder,
Your model is not properly constrained, you have rigid body motions, investigate your constraints, if you do not arrive to a conclusion port your model here and we will see what you are doing wrong, 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/

 

[Lunder]

Well, it seems to be the end caps that is not constrained properly. Tried several constraints on them now, but I dont find the right one. I have attached the .sim file so you can see what I have done.

Thanks!

 

[BlasMolero]

Dear Lunder,
Post the nastran input deck file, the one with the extension *.dat, as well as the *.log and *.f06 files, all are ASCII files, make a ZIP, the *.sim file is binary file and require to open to have the *.prt & *.fem file as well, and license of NX ADVANCED SIMULATION.
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/

 

[Lunder]

Here are the files:

http://www.filefactory.com/file/wcdey50c6qr/n/nastran_files_2_.zip

 

[BlasMolero]

Dear Lunder,
Here you are a few suggestions:
1.- Please, do not use solid tetraedral elements to mesh a vessel, Shell 2-D elements will give you extremely better results, perform a midsurface extraction in order to mesh with plate elements. If required to use solid edlements, please note you need at minimum TWO elements in the thickness, then the solid hexaedral CHEXA elements are preferred.
2.- GLUE surface-to-surface contact is designated to joint opposited surfaces, not the exterior faces of two solis, you have defined a contact Region 1 the outer surface of the cylindrical vessel and Region 2 the outer surface of the conical part. This is not correct, you need to define REGION 1 y 2 preciselly the contact faces of both cylindrical & conical parts.
3.- Your TET mesh is terrible distorted, you will arrive to useless results ...

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/

 

[Lunder]

Okey, thank you. But when I have done all that and try to solve, it says that "ERROR
Some elements in mesh "ThinShell(2):2d_mesh(2)" have missing nodal thicknesses in their
element associated data.
ACTION: Ensure that all elements in mesh have at least one non-zero nodal thickness value
defined or define a thickness value in the physical property of the mesh collector." I am not sure what to do now. I tried to go to physical properties, but could not find anything to make a change there.

 

[Lunder]

I figured it out. Thanks for all your input, BlasMolero!