The RSYS command seems to have no effect on the older element
formulations in a large deformation (NLGEOM,ON) analysis. Why?


This behavior is documented in Section 5.5.1 "Rotating Results
to a Different Coordinate System" in the ANSYS 8.1 Basic Analysis
Procedures Guide with the following note:

Note
In a large deformation analysis (for example, if you have issued the
NLGEOM ,ON command and the element has large deflection capability),
the element coordinate system is first rotated by the amount of rigid
body rotation of the element. Therefore the component stresses and
strains and other derived element data include the effect of the rigid
body rotation. The coordinate system used to display these results is
the specified results coordinate system rotated by the amount of rigid
body rotation. The exceptions to this are HYPER56, HYPER58, HYPER74,
HYPER84, HYPER86, and HYPER158. These elements always produce stresses
and strains in the specified results coordinate system (no rigid body
rotation added). This is also true for elements that contain hyperelastic
material properties (TB,HYPER), such as, SHELL181, PLANE182, PLANE183,
SOLID185, SOLID186, SOLID187, SHELL208, and SHELL209. For these elements,
when a hyperelastic material component is defined, the element component
result is always in the initial global coordinate system, regardless of
the coordinate system specified. For other (non-hyperelastic) material
properties, the output of the element component results is in the initial
global coordinate system (This is the default.). All component result
transformations to other coordinate systems will be relative to the
initial global system.

The primary data (for example, displacements) in a large deformation
analysis do not include the rigid body rotation effect, because the
nodal coordinate systems are not rotated by the amount of rigid body
rotation.

The note above is best explained by an example. The ANSYS 8.1 input
below compares the old generation elements (SOLID45 and SHELL43) to the
new generation elements (SOLID185 and SHELL181) for large deformation
(NLGEOM,ON) analyses. For RSYS,SOLU, both the old and new generation
elements give the stress and strain results in terms of the updated,
local element coordinate system, as one would expect.

However, the element behavior is different for RSYS,0. For the old
generation elements, the global Cartesian coordinate system rotates
(rigid body motion) along with the element, such that the results are
NOT in terms of the original global Cartesian system, but rather a
"new" global Cartesian system. If ESYS is not used for these old
elements, RSYS,0 and RSYS,SOLU will give the same results, so there
is no point to even requesting RSYS,0 results.

Conversely, the new generation elements are superior in that they give
RSYS,0 results in terms of the ORIGINAL global Cartesian coordinate
system, not some rotated system. Incidentally, if NLGEOM,ON is NOT
used, the old and new elements behave the same for RSYS,0 results,
since there is no update of the global Cartesian coordinate system.
The differences are only for large deformation analyses.


fini
/clear
/eshape,1
/view,,1,2,3
/plopts,info,1

/title, RSYS,0 Stress Results with NLGEOM,ON

/prep7
et,1,SOLID45
r,1
et,2,SOLID185,,2 ! enhanced strain formulation
r,2
et,3,SHELL43
r,3,0.1
et,4,SHELL181
r,4,0.1

mp,ex,1,30.0e6
mp,nuxy,1,0.30
mp,dens,1,0.00074
tb,biso,1
tbdata,1,60.0e3
tbdata,2,30.0e4

mat,1
esize,0.5
/dev,vect,1
/psym,esys,1

block,0,1,0,20,-0.05,0.05
type,1
real,1
lsel,u,loc,y,1,19
lesize,all,,,2
vmesh,1 ! 1st structure = SOLID45 (old generation brick)

block,2,3,0,20,-0.05,0.05
type,2
real,2
lsel,u,loc,y,1,19
lesize,all,,,2
vmesh,2 ! 2nd structure = SOLID185 (new generation brick)

rect,4,5,0,20
type,3
real,3
amesh,13 ! 3rd structure = SHELL43 (old generation shell)

rect,6,7,0,20
type,4
real,4
amesh,14 ! 4th structure = SHELL181 (new generation shell)

lsel,all
eplot
fini

/solu
antype,static
nlgeom,on
nsubst,10,1000,10
outres,all,all

nsel,s,loc,y,0.0
d,all,all,0.0
nsel,all

acel,0.0,0.0,386.4e2 ! 100 g load ...

eplot
solve
save
fini

/post1
set,last
/edge,,1
/dscale,,1
/dev,vect,0
plnsol,u,sum,2

rsys,0
nsel,s,loc,y,0.0,3.0
nsel,r,loc,z,0.0,0.1 ! top layer of brick elements ...
esln,s,1

/graph,full ! PowerGraphics does not support RSYS=SOLU
shell,top ! since PowerGraphics is not being used ...
/show,png

rsys,0
/title, RSYS=0 SY results
plnsol,s,y
rsys,solu
/title, RSYS=SOLU SY results
plnsol,s,y

rsys,0
/title, RSYS=0 SZ results
plnsol,s,z
rsys,solu
/title, RSYS=SOLU SZ results
plnsol,s,z
/show,close

/eof





.





Show Form
No comments yet. Be the first to add a comment!