Simmetric restrains

[Serchu]

Hi, is possible to add the option to include simmetric constrains (cero displacement/rotation in the normal plane) on the FEM workbench? Another way would be adding the possibility of select wich degree of freedom we want to restrain... here we could add a value, then if is adjust to cero is block and otherwise is an impossed displacement/rotation.


Best Regards

[bernd]

I already did some tests is this regard viewtopic.php?f=18&t=10331#p84593 I will need this for sure but at the moment I'm on other things.

Ahh I remember at the end I was struggling with CalculiX ...

... I don't know yet how that would work with element orientation not matching XYZ world coordinates.

That's the problem I've been struggling too. Even in CalculiX I don't know how this is done. Anyone around who knows how to define sloped constraints in CalculiX? If someone knows how to define spring constraints I'll be happy to know this too.

[Serchu]

One workaround by the moment could be define xyz restrain as usual but edit in the input file to leave just the normal direction to the simmetry plane.

Regards

[fandaL]

Hallo,
We need to define a local coordinate system and use it for a boundary conditions nodeset. I went through the ccx manual and it is viable.

1) for the chosen nodeset define a new coordinate system using card:
*TRANSFORM, name of nodeset
coordinates of point "a", coordinates of point "b"

Code: Select all

*TRANSFORM, NSET=FemConstraintFixed
0,0,1,  1,0,0

- local coordinate system has the origin in the [0, 0, 0] - same as global
- point "a" defines axis x' of local coordinate system from the origin
- point "b" defines the plane x'y' of local system (it lies anywhere in x'y' plane except axis x')
(figure is in the last link)

2a) define fixed directions as usual:

Code: Select all

*BOUNDARY
FemConstraintFixed,1

This will fix the displacement in direction 1 that is x' of local system which is in my case same as global z axis.
Calculix will use automatically local coordinate system, which is associated to "FemConstraintFixed" nodeset from above.

2b) and/or define displacement:

Code: Select all

*BOUNDARY
FemConstraintFixed,1,1, 0.1

FemConstraintFixed - is target nodeset
0.1 - means prescribed size of deformation
1,1 - means that it is in direction 1 that is x' (When I tried it, an analysis worked when 1 was written two times)

Details are in manual:
BOUNDARY:
http://web.mit.edu/calculix_v2.7/Calcul ... de163.html
TRANSFORM - see Figure.132
http://web.mit.edu/calculix_v2.7/Calcul ... de253.html