Warping Torsion shear stresses

SOFiSTiK Teddy
1

Dear all,
I have loaded a cantilever at the tip with a single torsional moment and activated warping torsion with ctrl warp 1 using version 2020. Now, for the given configuration, only shear stresses due to the torsional moment result at the restraint from torsion, the resultant of which represents the secondary torsional moment accordingly. In the Result Viewer, under unit shear stress from secondary torsional moment, it is of course correctly displayed how the stresses should run. However, if you look at the stresses in the Result Viewer under results - cross sections- stresses, the same sign appears both at the lower and upper flange (and slightly increased values, the difference between which, however, also corresponds to the stress bulge in the unit stresses, but I still cannot quite understand where the 0.11 comes from). The local sheet coordinate is shown by the arrows - can you give us an explanation for the discrepancies in these results? Code is inserted here, as as new member I can not attach any files…

Picture of the wrong stresses (at least according to my opinion): The shear stresses here should form the secondary torsional moment, but here they are outbalancing any torsional effects according to sign and stress direction.
Warp shear stress_2

################################################################
$Autor: Drilon Gubetini, ĂśberprĂĽfung WKT SOFiSTiK
+prog aqua urs:1
head Material und Querschnitt
NORM EN 1993-2005

STEE NO 1 TYPE S CLAS 355

SECT 1 MNO 1
PLAT YB 150[mm] ZB -207.5[mm] YE 0 T 15[mm]
PLAT YE -150[mm] T 15[mm]
PLAT YB 0[mm] ZB -200[mm] ZE 200[mm] T 10[mm]
PLAT YB 150[mm] ZB 207.5[mm] YE 0 T 15[mm]
PLAT YE -150[mm] T 15[mm]

WELD ZB -207.5[mm] YB 0 ZE -200[mm] T 0.003[m] mno 1
WELD ZB 207.5[mm] YB 0 ZE 200[mm] T 0.003[m] mno 1
END

+prog sofimsha urs:2
head System
syst 3D GDIV 1000 GDIR NEGZ

STO#L 5

$ Knoten
LOOP#I 126
NODE NO 1+#I X #I*#L/125 Y 0 Z 0
ENDLOOP

LOOP#I 125
BEAM NO 1+#I NA 1+#I NE 2+#I NCS 1
ENDLOOP

NODE NO 1 FIX F

END

+prog sofiload urs:3
head
LC NO 1
NODE NO 126 TYPE MXX 1 $-5.625

end

+prog ase urs:4
head
ctrl warp 1
lc 1
end

+prog aqb urs:5
head Vglspannungen
LC NO 1
stre smod e
end
############################################################################

Thanks in advance for your help
Best
Drilon

2

Hello Drilon

You are right, theoretically the shear stress should be 0 at the end of the flange. But here in SOFiSTiK the warping is constant along a beam element. Therefore, the stresses across a beam element are also constant. So if you let the element length tend to zero, you get the desired stress distribution.

grafik
grafik1297Ă—310 62 KB

(left: 51 nodes, middle: 151 nodes, right: 551 nodes)

The difference between the unit shear stress from secondary torsional moment and the shear stresses from aqb is that the shear stresses are calculated by adding the MTp, the MTs and the MTn. The sign is lost by adding the three parts of the torsional moments.

Further information can be found within the ase manual and the following TEDDY example.

SSD / TEDDY > Help > User Manuals > All Manuals… > ase > chapter 2.2.3 Warping torsion
TEDDY > File > Examples > ase > english > geometric_nonl >warping_mtp_mts_mtn.dat

If you want to understand the individual stress components due to warping, I recommend taking a look at the tool Beam 7 from the University of Innsbruck.
https://www.uibk.ac.at/stahlbau/software/index.html.de

Best regards
Frederik Höller
Your SOFiSTiK Support Team

1 Like
3

Hello Frederik,

thanks for your answer. The addition in aqb was the answer I needed.

Best
Drilon

1 Like