## Question about beam calculation with calculix

About the development of the FEM module/workbench.

Moderator: bernd

ickby
Posts: 2936
Joined: Wed Oct 05, 2011 7:36 am

### Question about beam calculation with calculix

Hello,

I'm calculating simple beam structures to analyse deformation and stress in profiles. The calculix solver has the option to choose 3d for output which allows for stress visualisation, compared to the 2d output. However, I also noticed different results dependent on that setting. For a very simple beam deformation is the same, no matter the output setting, but von mises stress is different. The "output 3D" value is correct according to normal beam theory, and the value for output=2d is wrong. Any idea why?

Example the file attached:

Deformation: 0.37mm
Stress 3d: ~6.3MPa (theory: 6.4MPa)
Stress 2d: ~0.73MPa
Beam.FCStd
Posts: 1479
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

### Re: Question about beam calculation with calculix

mmhh..there seems an issue with the model itself.
The tangent at the deflection-line should be zero at points A+B (the fixings), but that is not the case.
You can check it with paraview (convert frd-results to vtk-format, use "plot over line")
For this model the momentum-fixing is too "soft" (it rotates), you underestimate the moment at the fixing
and overestimate the bending-moment in the field.
beam_1D_example.JPG (101.7 KiB) Viewed 354 times
bernd
Posts: 9017
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

### Re: Question about beam calculation with calculix

but they are fixed ...

Code: Select all

``````***********************************************************
** Fixed Constraints
** written by write_constraints_fixed function
** ConstraintFixed001
*BOUNDARY
ConstraintFixed001,1
ConstraintFixed001,2
ConstraintFixed001,3
ConstraintFixed001,4
ConstraintFixed001,5
ConstraintFixed001,6``````
BTW: Stefan ... quite a lot of nodes ... Normally 1/10 of them would even be faily much.
bernd
Posts: 9017
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

### Re: Question about beam calculation with calculix

might be related to this issue #3056
UR_
Posts: 1153
Joined: Tue Jan 03, 2017 8:42 pm

### Re: Question about beam calculation with calculix

Got this:

Screenshot 003.png (18.81 KiB) Viewed 327 times

ickby
Posts: 2936
Joined: Wed Oct 05, 2011 7:36 am

### Re: Question about beam calculation with calculix

UR_ wrote:
Thu Jan 09, 2020 11:55 am
Got this:
Also when changing the analysis to 2d output and a rerun?
bernd
Posts: 9017
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

### Re: Question about beam calculation with calculix

ickby wrote:
Thu Jan 09, 2020 6:20 am

Deformation: 0.37mm
Stress 3d: ~6.3MPa (theory: 6.4MPa)
Stress 2d: ~0.73MPa

Beam.FCStd
confirmed for

OS: Windows 10 (10.0)
Word size of OS: 64-bit
Version: 0.19.19181 (Git)
Build type: Release
Branch: master
Hash: 2504247d65271b937dd5f033a0efff9c0d7bf375
Python version: 3.6.8
Qt version: 5.12.1
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: German/Switzerland (de_CH)

since the Displacement magnitude is 0.37 for both there really is something strange ...
bernd
Posts: 9017
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

### Re: Question about beam calculation with calculix

but to be honest I have no idea what are the von Mises for a 1D output? In which point in the cross section is this stress?
fandaL
Posts: 354
Joined: Thu Jul 24, 2014 8:29 am

### Re: Question about beam calculation with calculix

ickby wrote:
Thu Jan 09, 2020 6:20 am
Deformation: 0.37mm
Stress 3d: ~6.3MPa (theory: 6.4MPa)
Stress 2d: ~0.73MPa
FreeCAD reads nodal values of stress and displacement. CalculiX expands 1D and 2D elements to make analysis with 3D elements. If 2D output is requested, ccx interpolates values from 3D elements back to original 1D or 2D mesh. So if you have purely bent beam, interpolated stress will be ~0. And by the way if you have other than rectangular cross-section 3D representation is still hexa element so that nodal stresses cannot represent real cross-section.
But you can obtain integration point stresses in *.dat file by output request:

Code: Select all

``````*EL PRINT
S``````
maybe there is some tool to display them in Paraview.
You can also ask for beam forces and calculate stresses on your own according to your profile. I think it was discussed quite some time ago https://freecadweb.org/tracker/view.php?id=3126 . It should be card

Code: Select all

``````*EL FILE, SECTION FORCES
S``````
CalculiX will output beam forces instead of stresses. From manual *EL FILE card
• xx: Shear force in 1-direction
• yy: Shear force in 2-direction
• zz: Normal force
• xy: Torque
• xz: Bending moment about the 2-direction
• yz: Bending moment about the 1-direction
or use specialized sw for beam calculations...
bernd
Posts: 9017
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

### Re: Question about beam calculation with calculix

that makes sense ...

from calculix manual ...

Concerning the output, nodal quantities requested by the keyword *NODE PRINT are stored in the beam nodes. They are obtained by averaging the nodal values of the expanded element. For instance, the value in local beam node 1 are obtained by averaging the nodal value of expanded nodes 1, 4, 5 and 8. Similar relationships apply to the other nodes:

beam node 1 = average of expanded nodes 1,4,5 and 8
beam node 2 = average of expanded nodes 9,11,13 and 15
beam node 3 = average of expanded nodes 2,3,6 and 7

Screenshot_20200109_175255.png (19.13 KiB) Viewed 241 times

### Who is online

Users browsing this forum: felixlee868, Jee-Bee and 5 guests