# Tangential displacement boundary conditions to nodes belonging to plane stress/strain elements?

Hello

Is there a way/method in CalculiX to apply tangential displacement boundary conditions to nodes belonging to plane stress/strain elements? *TRANSFORM seems not to support a non-rectangular local coordinate system.

Hello,

i have here an example where i use boundary condition with a global cylindrical system.
I’m not sure, if these is different to your local coordinate system ?

wbr dichtstoff

rotating_ring_2D_plane_element.fbd

## Test objective: rotating ring & axisymmetric stress

PNT p0 0.00000 0.00000 0.00000
PNT P001 100.00000 0.00000 0.00000
PNT P002 0.00000 100.00000 0.00000
PNT P003 0.00000 50.00000 0.00000
PNT P004 50.00000 0.00000 0.00000
PNT P005 -100.00000 0.00000 0.00000
PNT P006 -50.00000 0.00000 0.00000
PNT P007 0.00000 -100.00000 0.00000
PNT P008 0.00000 -50.00000 0.00000
LINE L001 P004 P001
LINE L002 P001 P002 p0
LINE L003 P002 P003
LINE L004 P003 P004 p0
LINE L005 P002 P005 p0
LINE L006 P005 P006
LINE L007 P006 P003 p0
LINE L008 P005 P007 p0
LINE L009 P007 P008
LINE L010 P008 P006 p0
LINE L011 P007 P001 p0
LINE L012 P004 P008 p0
GSUR A001 - BLEND + L004 + L001 + L002 + L003
GSUR A002 + BLEND + L003 - L007 - L006 - L005
GSUR A003 - BLEND - L006 + L008 + L009 + L010
GSUR A004 - BLEND - L009 + L011 - L001 + L012
SETA ldivr l L001 L003 L006 L009
COMP ldivr d
SETA ldivt l L002 L004 L005 L007 L008 L010 L011 L012
COMP ldivt d
flip all
DIV ldivr mult 20
DIV ldivt mult 20
ELTY all QU4S
MESH all
send all abq
plot e all

rotating_ring_2D_plane_element.inp

**
** Structure: ring
** Test objective: rotating ring & axisymmetric stress
** radial displ ri 1624 ro 1425 tang. stress 6820 rad stress (ANSYS 799734)

Model: rotation ring

*INCLUDE, INPUT=all.msh

*TRANSFORM,TYPE=C,NSET=Nall
0,0,0,0,0,1
*BOUNDARY
Nall,2,2,0

*MATERIAL,NAME=Steel

*ELASTIC
210000,0.3

*DENSITY
78.5

*SOLID SECTION, Elset=Eall, Material=steel

*STEP

*STATIC

Eall,CENTRIF,10,0,0,0,0,0,1

*NODE FILE,OUTPUT=3D
U,

*EL FILE
S,

*END STEP

2 Likes

Hello

Thanks @dichtstoff. Your reply was very useful. I figured out that tangential displacement boundary conditions can be applied to nodes belonging to plane stress elements. I confirmed this with a simple test case. My files are here.

The User’s Manual says in 8.124 *TRANSFORM that “a non-rectangular local coordinate system is not allowed in nodes which belong to plane stress, plane strain, or axisymmetric elements.” But apparently, a cylindrical local coordinate system can be applied to a set of nodes belonging to plane stress elements and boundary conditions can be applied to this set with it.

1 Like