BAR/BEAM element in Advanced Nonlinear Analysis
BAR/BEAM element in Advanced Nonlinear Analysis
(OP)
Hi!
I´m trying to model a preloaded bolt which connects two metal plates. The plates and bolt head/nut are 3d SOLID and bolt shank is a preloaded BAR/BEAM element which is conectid with spider curves to bolt head/nut.
Since there´s a contact between elements I have to use Advanced Nonlinear Analysis and it works as long as I use Elastic material for BAR/BEAM element. Solid elements are Nonlinear Plastic.
When I change the bolt shank material type from Elastic to Nonlinear Plastic, the simulation won´t run anymore. I get the following error message:
***ERROR: Invalid default material model for element group 4.
***ERROR: Only cross-sections of type RECTANGULAR or PIPE
may be used for materially non-linear analysis.
Any ideas?
The model file is attached.
Thanks,
Edin M.
I´m trying to model a preloaded bolt which connects two metal plates. The plates and bolt head/nut are 3d SOLID and bolt shank is a preloaded BAR/BEAM element which is conectid with spider curves to bolt head/nut.
Since there´s a contact between elements I have to use Advanced Nonlinear Analysis and it works as long as I use Elastic material for BAR/BEAM element. Solid elements are Nonlinear Plastic.
When I change the bolt shank material type from Elastic to Nonlinear Plastic, the simulation won´t run anymore. I get the following error message:
***ERROR: Invalid default material model for element group 4.
***ERROR: Only cross-sections of type RECTANGULAR or PIPE
may be used for materially non-linear analysis.
Any ideas?
The model file is attached.
Thanks,
Edin M.





RE: BAR/BEAM element in Advanced Nonlinear Analysis
RE: BAR/BEAM element in Advanced Nonlinear Analysis
i just need to run analysis which can handle both contact and preloaded bolt.
RE: BAR/BEAM element in Advanced Nonlinear Analysis
You have assigned non-linear plastic material model to the CBAR element used to simulate the bolt pre-loaded, then 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/
RE: BAR/BEAM element in Advanced Nonlinear Analysis
Regards.
RE: BAR/BEAM element in Advanced Nonlinear Analysis
CBAR/CBEAM elements in Advanced Nonlinear Analysis (SOL601) with NX NASTRAN only works with elastic and bilinear plastic material models. For bilinear plastic beam elements, PBARL or PBEAML with circular or rectangular cross sections must be used.
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/
RE: BAR/BEAM element in Advanced Nonlinear Analysis
RE: BAR/BEAM element in Advanced Nonlinear Analysis
RE: BAR/BEAM element in Advanced Nonlinear Analysis
This is basic in FEMAP, if you do not know this basic nonlinear features I suggest to request a training to your local FEMAP & NX NASTRAN distributor:
1.- As I told you before you need to setup a PBEAML property choosing a NASTRAN shape instead the STANDARD FEMAP shape, see image:
2.- For bi-linear stress-strain curve, simply in the Nonlinear tab in the Nonlinearity type select "Elasto-Plastic (Bi-linear)", and define the yield criterium togther with SIGYLD value. For the plasticity modulus "H" you can computed based in the Tangent Modulus ETAN, if unknow in general you can use ETAN = 10% OF ELASTIC MODULUS:
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/
RE: BAR/BEAM element in Advanced Nonlinear Analysis
I ve never used this NASTRAN cross section before. I guess that s what I was missing. I think it should work now. I m on holidays now, but will try that next week and let you know if it works.
Regards,
Ed
RE: BAR/BEAM element in Advanced Nonlinear Analysis
I changed my model´s property and material.
Analysis still won´t run if I use Nonlinear Elasto-Plastic material.
Attached is the model file. Bolt shank material is ID 2 (Nonlinear Elasto-Plastic) and property is ID 4 (Nastran ROD, PBEAML/PBARL).
The results can be obtained from linear elastic material for the shank.
After changing it to Nonlinear El-Pl., analysis doesn´t run anymore.
Regards,
Ed
RE: BAR/BEAM element in Advanced Nonlinear Analysis
I just found in Advanced Nonlinear Theory and Modeling Guide that:
´´Both small and large displacement formulations can be used for
the bolts beam elements. Any cross-section available for the beam
element can be used, but only the isotropic elastic material model
can be used.´´
I removed bolt preload from the shank and the analysis runs now with nonlinear material. So I will just have to model the preload in a different way, e.g. axial load on the shank.
Thanks everyone.
Regards,
Ed
RE: BAR/BEAM element in Advanced Nonlinear Analysis
Here you are the manuals of NX NASTRAN Advanced Nonlinear Module (SOL601):
Best rgards,
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/
RE: BAR/BEAM element in Advanced Nonlinear Analysis
Also please note the WARNING written in the *.F06 file:
***WARNING: First non-zero strain value set to 1.1190476190476E-03 in TABLES1= 1 used in MATS1= 3.
((Yield stress)/(Youngs modulus))
In your second point of stress-strain function defined in FEMAP the value for STRAIN do not fully match the relation SIGYLD/EX = 2.35e8/2.1e11 = 0.001119, see copy of your function, then NX NASTRAN complaints with the above message:
0. 0.
0.00114 235000000.
0.01254 282000000.
0.1368 435000000.
0.14364 435000000.
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/
RE: BAR/BEAM element in Advanced Nonlinear Analysis
Can somebody, please, explain why the top bolt is moving out of the hole? That´s happening to two other bolts on the other side of the part. The simulation runs without errors (but stresses in all parts are negligible so I guess there´s some problem in analysis). Bolts have following constraints: TX, RX, RY, RZ. See attached animation.
Thanks,
Ed
RE: BAR/BEAM element in Advanced Nonlinear Analysis
It seems that contact is not performed correctly, revise the contact definition there, whitout the model at hand is difficult to tell you anything more definitive.
You mention something about applying constraints in the bolts: please note bolts should not have any EXTERNAL constraints, contact is an internal condition that will couple all parts, not neccesary to presscribe any global constraint, you will alterate the real behaviour of the structure.
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/
RE: BAR/BEAM element in Advanced Nonlinear Analysis
Thanks for replying. The contact has been set exactly the same way as in the previous simple model that we discussed before.
I will attach the new model here.
Regards,
Ed