Continue to Site

Eng-Tips is the largest engineering community on the Internet

Intelligent Work Forums for Engineering Professionals

Register Log in
  • Congratulations cowski on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!

BAR/BEAM element in Advanced Nonlinear Analysis 1

Status
Not open for further replies.
edinmer

edinmer

Mechanical
Apr 5, 2012
12
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.
 
Replies continue below

Recommended for you

Sort by date Sort by votes
not sure about your error, but be aware that the 3D elements for the head and nut are not transferring moment into the shank ('cause 3D elements only have translational freedoms. this might not be a concern, but if you're going to the trouble of using 3D elements for the head/nut, well, there could be some bending in the shank ... or maybe it's more that representing the shank as an ideal point and having the head bending about it's CL rather than being supported by the finite size of the shank ...
 
Upvote 0 Downvote
thanks for reply, but that's not an issue. i am aware of everything. the bolt shank will be just axially loaded and i want to avoid contact between shank and the hole in plates.
i just need to run analysis which can handle both contact and preloaded bolt.
 
Upvote 0 Downvote
Hello!,
You have assigned non-linear plastic material model to the CBAR element used to simulate the bolt pre-loaded, then the error.

deform_nonlin.png


Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran:
 
Upvote 0 Downvote
Thanks, I know that, but it should be possible to use non-linear plastic material for BEAM (not BAR - maybe in this model it's BAR element, but it doens+t work with BEAM either) element in Advanced Nonlinear Analysis. I have to do that because I'm modeling 10.9 bolt material. This here is just a test model.
Regards.
 
Upvote 0 Downvote
Hello!,
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.

cbar_cbeam_nolinear_sections_sol601.png


Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran:
 
Upvote 0 Downvote
surely the bolt shank (being modelled by the BAR) is a round section ?
 
Upvote 0 Downvote
Yes, I found that in the Advanced Nonlinear manual, but how to set that up? I made a BEAM element property with CIRCULAR BAR cross-section and it doesn't work. And how to set up the bilinear plastic material?
 
Upvote 0 Downvote
Hello 1984!,

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:

nastran_pbeaml.png


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:

bi-linear_nonlinear_material.png


Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran:
 
Upvote 0 Downvote
Thanks a lot, BlasMolero.
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
 
Upvote 0 Downvote
Hi!
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
 
 http://files.engineering.com/getfile.aspx?folder=3da76b81-4edf-45b3-be65-d8fe1aa04054&file=vijak_ploce_12.MOD
Upvote 0 Downvote
UPDATE:
I just found in Advanced Nonlinear Theory and Modeling Guide that:
´´Both small and large displacement formulations can be used for
the bolt’s 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
 
Upvote 0 Downvote
Hello!,
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: Blog de FEMAP & NX Nastran:
 
Upvote 0 Downvote
Hi!
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
 
 http://files.engineering.com/getfile.aspx?folder=8a11a788-495b-45e8-90a4-952e98ce0451&file=connection.gif
Upvote 0 Downvote
Dear Ed,
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: Blog de FEMAP & NX Nastran:
 
Upvote 0 Downvote
Status
Not open for further replies.

Similar threads

nl12345
  • Question
Using CBUSH Elements in GAP Element Connections
Replies
7
Views
3K
BlasMolero
BlasMolero
Xprivate
  • Question
Element Quality Check on FEMAP
Replies
0
Views
842
Xprivate
Xprivate
hhcc_im
  • Locked
  • Question
Failed for full nonlinear analysis after FEMAP export the analysis input file from working model
Replies
1
Views
937
BlasMolero
BlasMolero
D
  • Question
MODAL ANALYSIS WITH FLUID
Replies
3
Views
2K
karachun
karachun
manees90
  • Locked
  • Question
Modeling curved beam in femap 1
Replies
10
Views
710
manees90
manees90

Part and Inventory Search

Sponsor

Back
Top Bottom