Question about beam calculation with calculix

[ickby]

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

(115.05 KiB) Downloaded 73 times

[thschrader]

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 2842 times

[bernd]

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]

might be related to this issue #3056

[UR_]

Got this:

Screenshot 003.png (18.81 KiB) Viewed 2815 times

[ickby]

Got this:

Also when changing the analysis to 2d output and a rerun?

[bernd]

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
Word size of FreeCAD: 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]

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]

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]

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 2729 times