Analytical and theoretical values do not match

Hi,
I have a question for you.
I would be glad if you could answer my questions.

This program is based on a steel I-girder with a load in the y-axis direction applied to the center of the I-girder.
However, the Y-axis displacement of the focus point (Node Number: 60051) differs between the analytical value (0.11mm) and the theoretical value (0.022mm).
Where are the errors in this program?

Here is the analysis code


+PROG AQUA urs:1
HEAD U
UNIT TYPE 7
ECHO MAT
PAGE LANO 1 UNIO 7 UNII 7
MATE NO 1 E 210000 MUE 0.3
END

+PROG SOFIMSHA urs:2
HEAD U
PAGE LANO 1 UNIO 7 UNII 7
SYST REST ; CTRL REST 2 ; CTRL OPTI 50
SYST SPAC GDIR YY GDIV 100000

LET#A 0
LET#B 0
LOOP 101
NODE NO X Y=0 Z=0
1+#A 0+#B
LET#A #A+1
LET#B #B+50
ENDLOOP

TRAN TYPE NODE FROM 1 TO 101 INC 1 DNO 1000 DY -22

LET#A 0
LOOP 5
TRAN TYPE NODE FROM 1+#A TO 101+#A INC 1 DNO 10000 DZ 50
TRAN TYPE NODE FROM 10001+#A TO 10101+#A INC 1 DNO 1000 DY -22
LET#A #A+10000
ENDLOOP

TRAN TYPE NODE FROM 50001 TO 50101 INC 1 DNO 10000 DZ 44
TRAN TYPE NODE FROM 60001 TO 60101 INC 1 DNO 1000 DY -22
TRAN TYPE NODE FROM 60001 TO 60101 INC 1 DNO 10000 DZ 12
TRAN TYPE NODE FROM 70001 TO 70101 INC 1 DNO 1000 DY -22
TRAN TYPE NODE FROM 70001 TO 70101 INC 1 DNO 10000 DZ 44
TRAN TYPE NODE FROM 80001 TO 80101 INC 1 DNO 1000 DY -22

LET#A 0
LOOP 5
TRAN TYPE NODE FROM 80001+#A TO 80101+#A INC 1 DNO 10000 DZ 50
TRAN TYPE NODE FROM 90001+#A TO 90101+#A INC 1 DNO 1000 DY -22
LET#A #A+10000
ENDLOOP

LET#A 0
LOOP 14
TRAN TYPE NODE FROM 1+#A TO 101+#A INC 1 DNO 2000 DY -1978
TRAN TYPE NODE FROM 1001+#A TO 1101+#A INC 1 DNO 2000 DY -1978
LET#A #A+10000
ENDLOOP

LET#A 0
LET#B 0
LOOP 101
NODE NO X Y=-50 Z=294
150001+#A 0+#B
LET#A #A+1
LET#B #B+50
ENDLOOP

TRAN TYPE NODE FROM 150001 TO 150101 INC 1 DNO 20000 DZ 12

LET#B 0
LOOP 2
LET#A 0
LOOP 38
TRAN TYPE NODE FROM 150001+#A+#B TO 150101+#A+#B INC 1 DNO 200 DY -50
LET#A #A+200
ENDLOOP
LET#B #B+20000
ENDLOOP

$$ BRIC $$

LET#B 0
LOOP 13
LET#A 0
LOOP 100
BRIC N1 N2 N3 N4 N5 N6 N7 N8 MNO=1
1+#A+#B 1001+#A+#B 1002+#A+#B 2+#A+#B 10001+#A+#B 11001+#A+#B 11002+#A+#B 10002+#A+#B
LET#A #A+1
ENDLOOP
LET#B #B+10000
ENDLOOP

LET#B 0
LOOP 13
LET#A 0
LOOP 100
BRIC N1 N2 N3 N4 N5 N6 N7 N8 MNO=1
2001+#A+#B 3001+#A+#B 3002+#A+#B 2002+#A+#B 12001+#A+#B 13001+#A+#B 13002+#A+#B 12002+#A+#B
LET#A #A+1
ENDLOOP
LET#B #B+10000
ENDLOOP

LET#A 0
LOOP 100
BRIC N1 N2 N3 N4 N5 N6 N7 N8 MNO=1
61001+#A 150001+#A 150002+#A 61002+#A 71001+#A 170001+#A 170002+#A 71002+#A
LET#A #A+1
ENDLOOP

LET#B 0
LOOP 100
LET#A 0
LOOP 38
BRIC N1 N2 N3 N4 N5 N6 N7 N8 MNO=1
150001+#A+#B 150201+#A+#B 150202+#A+#B 150002+#A+#B 170001+#A+#B 170201+#A+#B 170202+#A+#B 170002+#A+#B
LET#A #A+200
ENDLOOP
LET#B #B+1
ENDLOOP

LET#A 0
LOOP 100
BRIC N1 N2 N3 N4 N5 N6 N7 N8 MNO=1
157601+#A 62001+#A 62002+#A 157602+#A 177601+#A 72001+#A 72002+#A 177602+#A
LET#A #A+1
ENDLOOP

$$ FIX$$

LET#A 0
LOOP 14
NODE 1+#A FIX PP,ZM
NODE 101+#A FIX XP,ZM
LET#A #A+10000
ENDLOOP

END

+PROG SOFILOAD urs:3
HEAD U
PAGE UNII 7 UNIO 7

LET#A 1
LOOP 11
LC #A
LINE REF VGRP TYPE pyy P1 100000 X1 0+500*(#A-1) Y1 -2000 Z1 0 $$
P2 100000 X2 0+500*(#A-1) Y2 -2000 Z2 600
LET#A #A+1
ENDLOOP

END

+PROG ASE urs:4
HEAD U
PAGE UNIO 7 UNII 7

loop 0
LET#A 0
LOOP 11
LC 1+#A
LET#A #A+1
ENDLOOP
endloop

lc 6

END

H.dat (3.1 KB)

Hello,

The reason for the differences in the results are the different calculation theories.
In your hand calculation you have used the Euler-Bernoulli beam theory. This has the consequence that the shear deformation of the cross-section is not taken into account.
If you work with continuum elements (BRIC), the shear deformations are taken into account. The same effect occurs when you work with beam elements in SOFiSTiK.

In your example you have defined a relatively short beam with a rather large cross-section (ratio h / L). As a result, the effect of shear deformations is large and the differences between your hand calculation and the FE results are quite large.

However, you can deactivate the effect of the shear deformations for a cross-section (see section No.3, open this section in the Cross Section Editor and check the Properties tab). As you can see in the next picture, the deformations in the middle of the beam are indentical to your hand calculation.

Project files:
Vergleich BEAM.sofistik (41.3 KB)
Vergleich BEAM.dwg (54.4 KB)
vergleich beam.gra (1.7 KB)

If you need further information about the so called Timoshenko beam theory, you can check out the following link or our AQUA (page 3-176, 2023) and ASE manual (2 Theoretical Principles).

If you want to know how you can deactivate the effects of the shear deformation, you can look at our online bridge design tutorial.

Best regards
Frederik Höller
Your SOFiSTiK Support Team

Thank you Frederick.

I understand that the difference in the calculations appears in whether or not shear deformation is taken into account.
I watched the video to get how to nullify shear deformation, but in the video, the analytical model is created in sofiPLUS.
I always use TEDDY’s text editor to create analytical models, so I did not understand how to nullify shear deformation.
So I would appreciate it if you could tell me how to disable shear deformation in the text editor.

If you are using bric/shell elements for your beam:
You can’t, your model has too much detail.

If you are using a beam element:

  • Define the section in AQUA
  • Set Ay/Az/Ayz/CMS to zero with the SV command