Example for 1D analysis

[bernd]

Does this picture show the postprocessed results of analysis carried out on 1D elements ? So it's possible to not only render beam profile but also display contour results on it ?

yes it is the way Calculix does 1D analysisi. It internally expands it to solid analysis. Thus with a preference it is possible to get the full solid mesh with was used internally by CalculiX to analyse the 1D element. Thus Calculix is restricted to only a few cross sections for 1D beam analysis. With the pref you can decide if you wish to have beam results or full solid results.

see post https://forum.freecadweb.org/viewtopic. ... 10#p520101

[NewJoker]

Does this picture show the postprocessed results of analysis carried out on 1D elements ? So it's possible to not only render beam profile but also display contour results on it ?

yes it is the way Calculix does 1D analysisi. It internally expands it to solid analysis. Thus with a preference it is possible to get the full solid mesh with was used internally by CalculiX to analyse the 1D element. Thus Calculix is restricted to only a few cross sections for 1D beam analysis. With the pref you can decide if you wish to have beam results or full solid results.

see post https://forum.freecadweb.org/viewtopic. ... 10#p520101

I know that CalculiX uses "fake" shell elements (shells are expanded to solids by the solver) but I didn't know that's the case with beam elements too. I thought that in CalculiX it's possible to define arbitrary cross-section for beam elements by providing the necessary section properties (area, moments of inertia, torsional constant) as it can be done in other software. Is there any workaround for that or can nothing be done to bypass this limitation ?

[twangrt]

I know that CalculiX uses "fake" shell elements (shells are expanded to solids by the solver) but I didn't know that's the case with beam elements too. I thought that in CalculiX it's possible to define arbitrary cross-section for beam elements by providing the necessary section properties (area, moments of inertia, torsional constant) as it can be done in other software. Is there any workaround for that or can nothing be done to bypass this limitation ?

You can set user defined beam elements in Calculix, tough it is not supported in FreeCAD.

Copy-paste from the Calculix manual:

Code: Select all

6.3.3 General
The general section can only be used for user element type U1 and is defined
by the following properties (to be given by the user in that order):
• cross section area A
• moment of inertia I11
• moment of inertia I12
• moment of inertia I22
• Timoshenko shear coefficient k

[NewJoker]

You can set user defined beam elements in Calculix, tough it is not supported in FreeCAD.

Copy-paste from the Calculix manual:

Code: Select all

6.3.3 General
The general section can only be used for user element type U1 and is defined
by the following properties (to be given by the user in that order):
• cross section area A
• moment of inertia I11
• moment of inertia I12
• moment of inertia I22
• Timoshenko shear coefficient k

Right, I've found some descriptions of those general beam sections. It seems that they are not hard to define, even though they require the definition of user element (subroutines seem unnecessary here). According to one user, they may provide strange results though.

Anyway, I wonder if we could add this feature to FreeCAD. It would be very useful and maybe not so difficult to implement.

[bernd]

As allways with any new feature in the regard of a solve. We need to know what we would like to implement, thus we need a working solver input file which has the new feature and runs with the solver.

[NewJoker]

As allways with any new feature in the regard of a solve. We need to know what we would like to implement, thus we need a working solver input file which has the new feature and runs with the solver.

Here's an exemplary input file with this feature: http://www.feacluster.com/CalculiX/ccx_ ... erbeam.inp

I submitted it in CalculiX and checked the results. They are correct - there's a good agreement with the deflection obtained in Abaqus and the one from simplified hand calculation.

[bernd]

added examples for the existing cross sections ... git commit f7cefaef475c553

there is a problem with the rectangle section ... Can someone explain the parameter of the third line from the Calculix beam section command? I assume the problem is there.

Code: Select all

*BEAM SECTION, ELSET=M0B0RstdD0, MATERIAL=MechanicalMaterial, SECTION=RECT
1250,400
-0, 1, 0

Code: Select all

** written by FreeCAD inp file writer for CalculiX,Abaqus meshes
** highest dimension mesh elements only.

** Nodes
*Node, NSET=Nall
1, 0, 500, 500
2, 8000, 500, 500
3, 1600, 500, 500
4, 3200, 500, 500
5, 4800, 500, 500
6, 6400, 500, 500
7, 800, 500, 500
8, 2400, 500, 500
9, 4000, 500, 500
10, 5600, 500, 500
11, 7200, 500, 500


** Edge elements
*Element, TYPE=B32, ELSET=Eedges
1, 1, 7, 3
2, 3, 8, 4
3, 4, 9, 5
4, 5, 10, 6
5, 6, 11, 2

** Define element set Eall
*ELSET, ELSET=Eall
Eedges



***********************************************************
** Element sets for materials and FEM element type (solid, shell, beam, fluid)
*ELSET,ELSET=M0B0RstdD0
1,
2,
3,
4,
5,

***********************************************************
** constraints fixed node sets
** ConstraintFixed
*NSET,NSET=ConstraintFixed
1,

***********************************************************
** Materials
** see information about units at file end
** FreeCAD material name: Calculix-Steel
** MechanicalMaterial
*MATERIAL, NAME=MechanicalMaterial
*ELASTIC
210000,0.3

***********************************************************
** Sections
*BEAM SECTION, ELSET=M0B0RstdD0, MATERIAL=MechanicalMaterial, SECTION=RECT
1250,400
-0, 1, 0

***********************************************************
** At least one step is needed to run an CalculiX analysis of FreeCAD
*STEP
*STATIC


***********************************************************
** Fixed Constraints
** ConstraintFixed
*BOUNDARY
ConstraintFixed,1
ConstraintFixed,2
ConstraintFixed,3
ConstraintFixed,4
ConstraintFixed,5
ConstraintFixed,6


***********************************************************
** constraints force node loads
*CLOAD
** ConstraintForce
** node load on shape: CantileverLine:Vertex2
2,3,-9.0000000000000E+06



***********************************************************
** Outputs --> frd file
*NODE FILE, OUTPUT=2d
U
*EL FILE
S, E
** outputs --> dat file
** reaction forces for Constraint fixed
*NODE PRINT, NSET=ConstraintFixed, TOTALS=ONLY
RF


***********************************************************
*END STEP 

***********************************************************
** CalculiX Input file
**   written by    --> FreeCAD 0.20.25427 (Git)
**   written on    --> Tue Aug  3 20:07:08 2021
**   file name     --> calculix-canti-rect.FCStd
**   analysis name --> Analysis
**
**
***********************************************************
**  About units:
**  See ccx manual, ccx does not know about any unit.
**  Golden rule: The user must make sure that the numbers he provides have consistent units.
**  The user is the FreeCAD calculix writer module ;-)
**
**  The unit system which is used at Guido Dhondt's company: mm, N, s, K
**  Since Length and Mass are connected by Force, if Length is mm the Mass is in t to get N
**  The following units are used to write to inp file:
**
**  Length: mm (this includes the mesh geometry)
**  Mass: t
**  TimeSpan: s
**  Temperature: K
**
**  This leads to:
**  Force: N
**  Pressure: N/mm^2 == MPa (Young's Modulus has unit Pressure)
**  Density: t/mm^3
**  Gravity: mm/s^2
**  Thermal conductivity: t*mm/K/s^3 == as W/m/K == kW/mm/K
**  Specific Heat: mm^2/s^2/K = J/kg/K == kJ/t/K
**

calculix-canti-rect.FCStd

(14.78 KiB) Downloaded 49 times

Screenshot_20210803_200845.png (200.06 KiB) Viewed 1654 times

[fandaL]

Can someone explain the parameter of the third line from the Calculix beam section command?

It is orientation of the cross section. Manual says under the *BEAM SECTION:

Second line:
• thickness in 1-direction
• thickness in 2-direction
Third line:
• global x-coordinate of a unit vector in 1-direction (default:0)
• global y-coordinate of a unit vector in 1-direction (default:0)
• global z-coordinate of a unit vector in 1-direction (default:-1)

You need to use
Model → Element geometry → Beam rotation
and rotate the profile. ATM you need to use 3D output to see the orientation. Even from Beam rotation tool user doesn’t see what is the rotated position.

[bernd]

now I have understood what 1-direction means ... I had been reading the manual for ten times no successs. After your post it is very obvisious for me what this 1-direction means ...

[bernd]

I am getting old ... I have spending time on this already an just forgot about it .... https://forum.freecadweb.org/viewtopic.php?t=24878

UR_ has explained it very well https://forum.freecadweb.org/viewtopic. ... 78#p195214