Nonlinear Static analysis + parabolic shell elements

[GruntCZ]

Hi!
I am trying to conduct a nonlinear analysis with shell elements. Is there a way, how to do that with parabolic shells? With, linear elements everything works nicely, but with parabolic elements results is same as results from standart static analysis.
Can anyone help me? please

 

[BlasMolero]

Dear Gruntcz,
The nonlinear element library of NX NASTRAN (SOL106) consists of the following element types:

•CBUSH and CBUSH1D for generalized nonlinear springs and dampers.
•CROD, CONROD, and CTUBE for unidirectional truss members.
•CBEAM for axially and laterally deforming line members.
•CQUAD4 and CTRIA3 for membrane, plate and shell modeling and hyperelastic plane strain.
•CQUAD8, CQUAD, and CTRIA6 for hyperelastic plane strain.
•CQUADX and CTRIAX for hyperelastic axisymmetric modeling.
•CHEXA, CPENTA, CPYRAM, and CTETRA for solid modeling.
•CGAP and slideline contact (BCONP, BLSEG, BFRIC, BWIDTH) for contact and friction modeling.

More in detail:
• 2-D Shell CQUAD4 are nonlinear elements for small strain analysis that can handle material or geometric nonlinearities or both. In geometric nonlinear analysis, these elements may undergo large total displacements and rotations but the net deformation of each element has to remain small, therefore these elements are called “small strain” elements. The element net rotation should not exceed 20 degrees and the element should not be stretched by more than 10%. If stretches exceed 20%, it is recommended to use hyperelastic elements if applicable.
• The hyperelastic elements are fully nonlinear finite deformation elements, including large strain and large rotation. The following elements are available: plane strain (CQUAD4, CQUAD8, CQUAD, CTRIA3, and CTRIA6), solid (CHEXA, CPENTA, and CTETRA) and axisymmetric elements (CQUADX and CTRIAX).

In summary, CQUAD8 high-order 8-nodes elements must be used to solve highly nonlinear hyperelastic plain strain/Axisymmetric problems. I will check with NX NASTRAN developers why not a written warning exist in the F06 when used in nonlinear small strain problems.

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/

 

[GruntCZ]

Thanks BlasMolero, for quick response

I am trying to solve a simple box (100x100x100 mm with 5 mm thick wall), with pressure on one side, and fix BC on the opposit side. It's a testing job, for a much complex calculation of reservoir with internal pressure. I tried to use the plane strain element to solve my problem, but results seems to be completely wrong. With linear plate elements, static and non-liner static seems to work fine. I am finding the whole theory of plane strain unusable for vessels with internal pressure.
Do you have any suggestions which type of elements I am supposed to use? Whole reservoir is approximately 5 m high and made from 5 mm thick steel plates.

Thanks for any reply.

 

[BlasMolero]

Dear GruntCZ,
Use CQUAD4 plate elements, you don't need to use at all high-order CQUAD8 elements, you are not simulating a "metal-forming" problem, in this case you will need to run ADVANCED NONLINEAR Analysis (SOL601/701) solver.

The 4-nodes CQUAD4 elements are perfect for nonlinear "small strain" analysis to account for stress stiffening effects using BASIC nonlinear solver of NX NASTRAN (SOL106). The nonlinear element calculations are activated if a nonlinear material exists (MATS1 or CREEP Bulk Data entries) or if a geometric nonlinear analysis of the whole model is requested with PARAM,LGDISP,1.

Large strain effects are pronounced in metal forming, rubber and elastomer applications. In such applications, the strains exceed 100%. Finite strain formulation is required to treat the problems in this category, then you need license for NX NASTRAN Advanced Nonlinear solver (SOL601/701).

NX Nastran Basic Nonlinear module (SOL106) supports the large strain capability for rubbers and elastomers. This formulation contains the effect of large strain as well as geometric nonlinearity. However, NX Nastran doesn’t support large strain formulation for metal forming applications. In most structural applications, however, moderately large strains (20 to 30%) appear in local areas if there is any large deformation.

Be practical, 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/

 

[GruntCZ]

Thanks for thorough reply.
So, the conclusion is, that I have to use common 4 node elements...?

 

[GruntCZ]

There is one more thing. Can you tell me where I can find the element library for NX Nastran, and its analysis types?

 

[BlasMolero]

In FEMAP go to HELP > NX NASTRAN

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[GruntCZ]

BlasMolero: thanks a lot