Reaction moment output from b32r element from fixed support location

Hi,

Is there a way to taking moment reaction from fixed support locations of b32r element? I can easily read reaction forces of fixed support locations from .dat file but I cannot find a way to take similar output format for moment reactions.

Regards,

Hi,

  • maybe you can change to a cylindrical coordinate systeme for your output
  • maybe you can use *section print

    wbr
1 Like

Thank you for your concern. I did not understand clearly that changing to cylindirical cordinates. Actually my main problem is, I cannot write outputs of moment reactions like writing reaction forces output of fixed support location.
As far as I know I can use *SECTION print command with only surface option. In my case, I have two beam(b32r) model like in the figure below. I appy a concentrated load on the intersection point of two beams and apply fix support on two ends.

*SECTION PRINT is indeed meant for output from faces but you can use *EL FILE, SECTION FORCES for beam elements.

1 Like

Thank you for your answer. I tried the *EL FILE,Output=3d, Output=2D, SECTION FORCES but, the moment reaction results differs with the ansys or other fea softwares even if reaction forces of fixed supports are both same with calculix and other fea softwares. I have taken the moment results from vtkpost and compare with the terminology which i shown you below.

there is an example in the user manual ccx,
these worked fine for me: here with differen load

*NODE,NSET=Nall
1, 0, 0, 0
2, 0, 0, 50
3, 0, 0, 100
*ELEMENT,TYPE=B32R,ELSET=EAll
1,1,2,3
*BOUNDARY
3,1,6
*MATERIAL,NAME=ALUM
*ELASTIC
1E7,.3
*BEAM SECTION,ELSET=EAll,MATERIAL=ALUM,SECTION=RECT
2.,2.
1.d0,0.d0,0.d0
*STEP
*STATIC
*CLOAD
1,1,1
1,2,5
1,3,10
*EL PRINT,ELSET=Eall
S
*NODE FILE, OUTPUT=2D
U
*EL FILE, SECTION FORCES
S,NOE
*END STEP

image

image

1 Like

Make sure that you are comparing the same components, units and locations (fixed node).

I guess I read moment reactions results from wrong place. I solved the simple beam model which you share here and read results from Vtkpost. The Vtkpost results are shown below.


I think I should compare this SZX value with? Could you correct me if am I wrong?

So is there an issue about transformation of output coordinates?

image

Yes I also shared this picture two posts before. Can we see moment reactions regarding to global coordinates?

maybe you have a coordinate system according of the direction of the beam,
you can test it by changing the cordinates of the nodes!?
you have to play and test some changes

Again it has not to be major changes in values? Because the reaction forces are calculated truly. The solution that you suggest will not work( even if i said that i tried and nothing changes). So it has to be different solution of the problem.

¿Is there any particular reason why ccx store those two different magnitudes inside the same variable “S”?

It seems impossible to print Stresses and Section Forces at the same time for the same analysis.

I have tried :

*EL FILE,OUTPUT=2D,SECTION FORCES

S,S,NOE

And

*EL FILE,OUTPUT=2D

S

*EL FILE,OUTPUT=2D,SECTION FORCES

S,NOE

But seems they are mutually exclusive. ¿Is there any workaround.?

CCX structural elements aren’t true structural elements but are created from brick elements, so there are only 3 translation degrees of freedom, no rotations. Some additional calculations are needed in order those elements being representative of a beam section (available for a limited number of cross sections). The output has to be requested with the key: *SECTION PRINT
Check the manual about this key: ccx_2.19.pdf (dhondt.de)

The number of predefined cross-sections is limited but it’s worth mentioning that there’s a user beam element which can have an arbitrary section defined by proper constants.

2 Likes

Thanks both,

It works and I can see some output printed on my *.dat file:


statistics for surface set S1 and time 0.1000000E+01
total surface force (fx,fy,fz) and moment about the origin(mx,my,mz)
-8.203642E-09 -7.319032E-09 -9.999600E+02 4.746009E-09 9.999931E+02 7.276014E-09
center of gravity and mean normal
0.000000E+00 0.000000E+00 -6.776264E-19 -1.000000E+00 0.000000E+00 .000000E+00
moment about the center of gravity(mx,my,mz)
4.746009E-09 9.999931E+02 7.276014E-09
area, normal force (+ = tension), shear force (size), torque and bending moment (size)
2.500000E-03 8.203642E-09 9.999600E+02 -4.746009E-09 9.999931E+02

The point is that I cannot get both simultaneously available in the GUI.

Manual says:

S [STRESS (real), STRESSI (imaginary)]: true (Cauchy) stress in structures. For beam elements this tensor is replaced by the section forces if SECTION FORCES is selected.

is replaced: I can only see one or the other with *EL FILE. Ideally, I would like to have both available in the GUI.

1 Like

Dear Disla,

Thank you for your answer. I could not understand clearly how can you get the force and moment values on the same screen with .dat file.
Could you please share what cards did you use to get this results? I can only see reaction forces in .dat file.
I am sharing my output commands below.
image

The stresses at the integration points are obtained by a *EL PRINT card,
the stresses at the nodes by the OUTPUT=3D option (default) on the *EL FILE
card, whereas for the section forces the SECTION FORCES option on the same
card is used (this option is mutually exclusive with the OUTPUT=3D option).
The displacements are best obtained in the non-expanded view, i.e. using the
OUTPUT=2D option. This means that for the present results the example
had to be run twice: once with the OUTPUT=3D option and once with the
SECTION FORCES option.

from Manual: 5.14 Cantilever beam using beam elements

@JuanP74

Thanks Juan.

@osmcnkrtn

*Node Print RF is for reaction forces only.

Use *SECTION PRINT as @JuanP74 and @dichtstoff has previously suggest.

*SECTION PRINT,SURFACE=S1,NAME=Forces_Moments
SOF,SOM

page 86 manual v2.20.

1 Like

Thanks Disla.
The problem is I have a beam model with b32 element, so there is no chance to define *SECTION PRINT, SURFACE… because the fixed support point is just a node not a surface.
I looked at the manual and cannot find *NODE PRINT card has a Moment reaction output option.Is there a way to write reaction moment of a fixed supported node or element with *SECTION FORCES or other options?
or alternative way
As I understand from the manual section forces of beams are written in local 1 and 2 cordinate system of the beam. Could we transfer these results to global cordinates and then see the results?
I guess in vtk post the SXY, SZX and SYZ are the moment reactions of node 1 but this values are calculated for local beam cordinate system. How can we turn these results to global cordinates?