Cancel
Showing results for 
Search instead for 
Did you mean: 

differences between CBEAM and CBAR

Genius
Genius

Hi,

 

I want to know the differences between CBEAM and CBAR on NX Nastran. I usually use two RB2 with a CBEAM for modeling bolt conections on CAE systems like Hypermesh. Which is the difference between CBEAM and CBAR for bolt conections?

 

Thanks.

4 REPLIES

Re: differences between CBEAM and CBAR

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Dear Igor,

• The CBAR element description, in Spanish:

http://www.iberisa.com/soporte/femap/cbar.htm

 

• The CBEAM element description, in Spanish:

http://www.iberisa.com/soporte/femap/cbeam.htm

 

Regarding differences, basically the CBAR element is a subset of the CBEAM element, a simplification. If you have a solid cross section and fully symmetric, then use CBAR. But if you have an open thin walled cross section, non symmetric, where you want to consider the warping effect, etc.., in summary a complex cross section, then CBEAM element is the one to use.

 

But my suggestion in such complex situation is ALWAYS to mesh using 2-D Shell CQUAD4 elements, to avoid surprises like not detecting the lateral buckling of the cross section, i.e., torsional buckling in structures supporting bending loadings with unsymmetrical cross sections, open profiles, thin walled, etc..

 

The CBAR element is a general purpose beam that supports tension and compression, torsion, bending in two perpendicular planes, and shear in two perpendicular planes. The CBAR uses two grid points and can provide stiffness to all six DOFs of each grid point. With the CBAR, its elastic axis, gravity axis, and shear center all coincide. The displacement components of the grid points are three translations and three rotations.

You define a CBAR element using the CBAR bulk data entry and define its properties using the PBAR bulk data entry.

 

CBAR

 

The CBEAM element includes extension, torsion, bending in two perpendicular planes, and the associated shear. The CBEAM element provides all of the capabilities of the CBAR element, plus the following additional capabilities:

  • You can define different cross-sectional properties at both ends and at up to nine intermediate locations along the length of the beam.

  • Τhe neutral axis and shear center don’t need to coincide, which is important for unsymmetrical sections.

  • The effect of cross-sectional warping on torsional stiffness is included (PBEAM only).

  • The effect of taper on transverse shear stiffness (shear relief) is included (PBEAM only).

  • The CBEAM lets you apply either concentrated or distributed loads along the beam, using the PLOAD1 entry.

  • You may include a separate axis for the center of nonstructural mass.

  • Distributed torsional mass moment of inertia is included for dynamic analysis.

  • The CBEAM lets you model a beam made up of offset rods, using the PBCOMP entry.

  • CBEAMs support nonlinear material properties: elastic perfectly plastic only (see TYPE = PLASTIC on MATS1 entry).

  • You can have separate shear center, neutral axis, and nonstructural mass center of gravity.

  • Arbitrary variation of the section properties (A, I1, 12, I12, J) and of the nonstructural mass (NSM) along the beam (PBEAM only).

 

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Re: differences between CBEAM and CBAR

Valued Contributor
Valued Contributor

Hi Blas,

As I have understood so far when CBEAM is defined, the Grid Points (GA, GB) line coincide with the shear center of the cross-section. 

 

Let me insert 3 images taken of CBEAM.

 

 

1.png

 

 

2.png

 

3.png

 

Picture 2 & 3 illustrate how Neutral Axis Offset option can be used. I understand the reasoning behind it i.e. physics.

 

My question is, if I have a section in which the Neutral Axis is not coincident with shear center, then should the offset value be supplied manually or will FEMAP calculate the offset values automatically based on the shape of cross-section?

 

If the answer is yes, FEMAP/Patran will calculate the Neutral axis offset automatically, then I have a follow up question. If I have a plate which has a C-Channel stiffener attached to it and if I model it in FEMAP such that, the C-Channel is modeled using offseted CBEAM elements, then if I supply the values of Wa & Wb respectively, will it be sufficient to get accurate representation of the structure?

 

I hope my wording isn't confusing.

 

Thx

Re: differences between CBEAM and CBAR

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Dear Nagaraj,

Take a look to this post & video, I hope that it will answer all your questions exactly:

 

https://iberisa.wordpress.com/2015/09/29/beam-cross-section-using-surface-with-reference-point-on-fe...

 

dimensiones-modelo.png

 

malla-shell-beam.png

 

In fact, you can use CBEAM elements to represent open sections, but caution!!: this is a global model, a global answer, nothing to see with the use of the Shell CQUAD4 element that allows you to perfectly capture thin cross section, open and no symmetric, and perform nos linear analysis for the geometry!!. Don't forget this, always make your double check using a detailed model with Shell elements, I am clear enough?.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Re: differences between CBEAM and CBAR

Valued Contributor
Valued Contributor

I am reviving this topic to provide futher information.

 

This excellent document put out by Siemens answers a few question I had on entry of shear center and/or Neutral Axis offset values in to CBEAM entry.

 

https://docs.plm.automation.siemens.com/data_services/resources/nxnastran/10/help/en_US/tdocExt/pdf/...

 

Refer to page 3-28 (54 in pdf file) for an example of Tapered Beam. 

 

The above example includes a dat file which I am trying to import in to FEMAP. After importing, I see no entities in Femap (same thing in patran as well). Is the dat file correct?

 

$ FILENAME - BEAM2.DAT
ID LINEAR,BEAM2
SOL 101
TIME 5
CEND
TITLE = TAPERED BEAM MODEL
DISP = ALL
STRESS = ALL
FORCE = ALL
LOAD = 1
SPC = 1
BEGIN BULK
PARAM POST 0
PARAM AUTOSPC YES
$
GRID 1 0.0 0.0 0.0
GRID 2 0.0 0.0 50.0
SPOINT 101 102
SPC 1 1 123456 0.0
CBEAM 1 11 1 2 0. 1. 0.
2.367 0. 0. 1.184 0. 0.
101 102
$$
2 3 4 5 6 7 8 9
$
PBEAM 11 21 12.000 56.000 17.000 3.930
-3.000 .867 -3.000 4.867 3.000 4.867 3.000 .867
YES .100 10.830 45.612 13.847 3.201
-2.850 .824 -2.850 4.624 2.850 4.624 2.850 .824
YES .200 9.720 36.742 11.154 2.579
-2.700 .780 -2.700 4.380 2.700 4.380 2.700 .780
YES .300 8.670 29.232 8.874 2.052
-2.550 .737 -2.550 4.137 2.550 4.137 2.550 .737
YES .400 7.680 22.938 6.963 1.610
-2.400 .694 -2.400 3.894 2.400 3.894 2.400 .694
YES .500 6.750 17.719 5.379 1.244
-2.250 .650 -2.250 3.650 2.250 3.650 2.250 .650
YES .600 5.880 13.446 4.082 .944
-2.100 .607 -2.100 3.407 2.100 3.407 2.100 .607
YES .700 5.070 9.996 3.035 .702
-1.950 .564 -1.950 3.164 1.950 3.164 1.950 .564
YES .800 4.320 7.258 2.203 .509
-1.800 .520 -1.800 2.920 1.800 2.920 1.800 .520
YES .900 3.630 5.124 1.556 .360
-1.650 .477 -1.650 2.677 1.650 2.677 1.650 .477
YES 1.000 3.000 3.500 1.062 .246
-1.500 .434 -1.500 2.434 1.500 2.434 1.500 .434
.241 -.666 0. 70.43 1.10
0. 2.367 0. 1.184
$
MAT1 21 3.+7 .3
$
FORCE 1 2 192. 0. 1. 0.
ENDDATA