Shear Stress in CBAR element under end in-plane torque load
Shear Stress in CBAR element under end in-plane torque load
(OP)
Hi all,
I am new to MSC.Nastran/Patran. I have modeled a beam along Z-Direction (one end is fixed and other end is free) with CBAR elements. The cross section of the beam is box-shaped. The free end is loaded with torque load(Mz - XY Plane). The problem is I am not able to get any stress results from. I also tried CBEAM but still I get no results.
Both CBAR and CBEAM have torsional (transverse shear) stiffness but they give no response in stress-wise. Is there any parameter or keyword to invoke shear stiffness? Do you have any tips about this?
http://www.aero.polimi.it/~lanz/bacheca/downloads/...
Thanks in advance,
(This is the .bdf file)
I am new to MSC.Nastran/Patran. I have modeled a beam along Z-Direction (one end is fixed and other end is free) with CBAR elements. The cross section of the beam is box-shaped. The free end is loaded with torque load(Mz - XY Plane). The problem is I am not able to get any stress results from. I also tried CBEAM but still I get no results.
Both CBAR and CBEAM have torsional (transverse shear) stiffness but they give no response in stress-wise. Is there any parameter or keyword to invoke shear stiffness? Do you have any tips about this?
http://www.aero.polimi.it/~lanz/bacheca/downloads/...
Thanks in advance,
(This is the .bdf file)
CODE -->
$ Direct Text Input for Nastran System Cell Section
$ Direct Text Input for File Management Section
$ Direct Text Input for Executive Control
$ Linear Static Analysis, Database
SOL 101
CEND
$ Direct Text Input for Global Case Control Data
TITLE = MSC.Nastran job created on 10-Aug-14 at 13:11:15
ECHO = NONE
SUBCASE 1
SUBTITLE=beamonlycase
SPC = 2
LOAD = 2
DISPLACEMENT(SORT1,REAL)=ALL
SPCFORCES(SORT1,REAL)=ALL
GPFORCE=ALL
STRESS(SORT1,REAL,MAXS,BILIN)=ALL
$ Direct Text Input for this Subcase
BEGIN BULK
$ Direct Text Input for Bulk Data
PARAM POST 0
PARAM PRTMAXIM YES
$ Elements and Element Properties for region : realbeam
PBARL 1 1 BOX
500. 300. 2. 2.
$ Pset: "realbeam" will be imported as: "pbarl.1"
CBAR 1 1 1 3 0. 1. 0.
CBAR 2 1 3 4 0. 1. 0.
CBAR 3 1 4 5 0. 1. 0.
CBAR 4 1 5 6 0. 1. 0.
CBAR 5 1 6 7 0. 1. 0.
CBAR 6 1 7 8 0. 1. 0.
CBAR 7 1 8 9 0. 1. 0.
CBAR 8 1 9 10 0. 1. 0.
CBAR 9 1 10 11 0. 1. 0.
CBAR 10 1 11 12 0. 1. 0.
CBAR 11 1 12 13 0. 1. 0.
CBAR 12 1 13 14 0. 1. 0.
CBAR 13 1 14 15 0. 1. 0.
CBAR 14 1 15 16 0. 1. 0.
CBAR 15 1 16 17 0. 1. 0.
CBAR 16 1 17 18 0. 1. 0.
CBAR 17 1 18 19 0. 1. 0.
CBAR 18 1 19 20 0. 1. 0.
CBAR 19 1 20 21 0. 1. 0.
CBAR 20 1 21 22 0. 1. 0.
CBAR 21 1 22 23 0. 1. 0.
CBAR 22 1 23 24 0. 1. 0.
CBAR 23 1 24 25 0. 1. 0.
CBAR 24 1 25 26 0. 1. 0.
CBAR 25 1 26 27 0. 1. 0.
CBAR 26 1 27 28 0. 1. 0.
CBAR 27 1 28 29 0. 1. 0.
CBAR 28 1 29 30 0. 1. 0.
CBAR 29 1 30 31 0. 1. 0.
CBAR 30 1 31 32 0. 1. 0.
CBAR 31 1 32 33 0. 1. 0.
CBAR 32 1 33 34 0. 1. 0.
CBAR 33 1 34 35 0. 1. 0.
CBAR 34 1 35 36 0. 1. 0.
CBAR 35 1 36 2 0. 1. 0.
$ Referenced Material Records
$ Material Record : steel
$ Description of Material : Date: 10-Aug-14 Time: 13:02:58
MAT1 1 7.86-9 .3
$ Nodes of the Entire Model
GRID 1 0. 0. 0.
GRID 2 0. 0. 3500.
GRID 3 0. 0. 100.
GRID 4 0. 0. 200.
GRID 5 0. 0. 300.
GRID 6 0. 0. 400.
GRID 7 0. 0. 500.
GRID 8 0. 0. 600.
GRID 9 0. 0. 700.
GRID 10 0. 0. 800.
GRID 11 0. 0. 900.
GRID 12 0. 0. 1000.
GRID 13 0. 0. 1100.
GRID 14 0. 0. 1200.
GRID 15 0. 0. 1300.
GRID 16 0. 0. 1400.
GRID 17 0. 0. 1500.
GRID 18 0. 0. 1600.
GRID 19 0. 0. 1700.
GRID 20 0. 0. 1800.
GRID 21 0. 0. 1900.
GRID 22 0. 0. 2000.
GRID 23 0. 0. 2100.
GRID 24 0. 0. 2200.
GRID 25 0. 0. 2300.
GRID 26 0. 0. 2400.
GRID 27 0. 0. 2500.
GRID 28 0. 0. 2600.
GRID 29 0. 0. 2700.
GRID 30 0. 0. 2800.
GRID 31 0. 0. 2900.
GRID 32 0. 0. 3000.
GRID 33 0. 0. 3100.
GRID 34 0. 0. 3200.
GRID 35 0. 0. 3300.
GRID 36 0. 0. 3400.
$ Loads for Load Case : beamonlycase
SPCADD 2 1
LOAD 2 1. 1. 1 1. 3
$ Displacement Constraints of Load Set : fixed
SPC1 1 123456 1
$ Nodal Forces of Load Set : load
FORCE 1 2 0 0. .57735 .57735 .57735
$ Nodal Forces of Load Set : load
MOMENT 3 2 0 100. 0. 0. -1.
$ Referenced Coordinate Frames
ENDDATA 5319d802 




RE: Shear Stress in CBAR element under end in-plane torque load
In fact, nastran do not compute at all neither shear or torsional stresses for cbar/cbeam elements, but not only nastran, in general any FEA codes of type "general purpose" do not compute shear/torsional stresses in bar/beam elements because the assumption for beam elements follows the beam theory where torsion and shear stresses are negligible in comparison with axial + bending combination stresses. If this is not true, then you should use other elements like plane & shell elements or solid elements (by the way, I read your model in FEMAP and it is not appropiate at all to use a CBAR element to represent a hole box cross section of 500x300 with very LOW thickness = 2.0!!. Not correct, if this is a real situation you must use plate CQUAD4 elements and run a nonlinear analysis to account for geometric nonlinear behaviour).
But fortunately for the FEMAP users we have THE BEAM CALCULATOR utility under the FEMAP postprocessor tools that is able to consider not only axial & bending forces in bar/beam elements but also shear & torsion forces coming from any FEA solver (nastran, ansys, abaqus, etc..) to compute not only vonMises stress but also axial, shear and principal stresses along the beam elements. To learn more take a look to this link:
http://iberisa.files.wordpress.com/2014/06/12_beam...
Best regards,
Blas.
~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director
IBERISA
48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog de FEMAP & NX Nastran: http://iberisa.wordpress.com/
RE: Shear Stress in CBAR element under end in-plane torque load
What I remeber from Ansys is, BEAM 188 element is capable to reflect shear stresses without any additional implementations. After your advise, I am gonna focus on FEMAP more deeply.