help on simply supported cylinder analysis

Hoi Ashraf


''Also i want to know how do we apply Moment(Mx) and normal force(Nx) as the boundary condition. i am finding the axial modes so i need to keep V = W = 0; Mx = Nx = 0'':

(Here I am not sure what you really want: ''V = W = 0; Mx = Nx = 0''. If you only suppress these dofs you have a rigid body movement in axial direction (as you can see in your mess file) but you wonot find the axial modes. The axial modes will be calculated also if you apply u=v=w=0 (at both edges) and maybe even rx=ry=rz=0.
If you want to suppress translations and rotations at both edges, put DX=DY=DY=DRZ=DRY=DRZ=0. Just try this and watch your results.
Note that although you are searching for axial modes, bending modes will occur as well, depending on the frequencies.)

For the ''boundary conditions'' you can use something along these lines:

[code:1]
Loaddyn=AFFE_CHAR_MECA(MODELE=model,
DDL_IMPO=(_F(GROUP_MA='edges',
DX=0.0, DY=0.0, DZ=0.0,
DRX=0.0,DRY=0.0,DRZ=0.0),);
[/code:1]

If you really need forces, use eg:

[code:1]
clamped=AFFE_CHAR_MECA(MODELE=model,
DDL_IMPO=(_F(GROUP_MA=('outedge',),
DX=0.0,
DY=0.0,
DZ=0.0,),),
#FORCE_COQUE=_F(GROUP_MA='shin', PRES=-1/Ain,),);
#FORCE_ARETE=_F(GROUP_MA='inedge', FZ=-1/Linside,),);
FORCE_NODALE=_F(GROUP_NO='node1', FZ=-1.0,),);
#FORCE_NODALE=_F(GROUP_NO='nodes13',FZ=-0.50,),);
#FORCE_NODALE=_F(GROUP_NO='nodes4', FX=-0.25,),);
[/code:1]
(For nodes connected to shell elements with rotational degrees of freedom, you can of course also use moments: use MX, MY, MZ (????) instead of FX, FY, FZ.)


You use as boundary conditions:

[code:1]
clamp=AFFE_CHAR_MECA(MODELE=modinit,
DDL_IMPO=_F(GROUP_MA='edges',
DX=0.0,
DY=0.0,),);
[/code:1]


So your construction will have rigid body modes (in z direction).
This may explain the error message:
la matrice de raideur est singulière malgre la strategie de décalage
(structure avec des modes de corps solide).

Although you *can* run mode shape analysis on a structure with rigid body movements, you may need another type of solution eg. band (donot recall the french CAster name right now).

In your linear static case, you use 'load','edges','surface' for COQUE, but, 'load' and 'edges' are no shells. They are just line elements (''beams'') and cannot be reoriented.

[code:1]
coque=AFFE_CARA_ELEM(MODELE=FEMLin,
COQUE=_F(GROUP_MA=('load','edges','surface',),
EPAIS=0.01,
COQUE_NCOU=1,),);

but use:

coque=AFFE_CARA_ELEM(MODELE=FEMLin,
COQUE=_F(GROUP_MA=('surface',),
EPAIS=0.01,
COQUE_NCOU=1,),);
[/code:1]




kind regards - kees<br /><br />Post edited by: Kees Wouters, at: 2010/06/21 23:14

Hoi Ashraf

about the static case: I guess you want to supply a radial force on all the nodes in the group 'load' (or a distributed radial force on the beams corresponding to these nodes). Is this assumption correct? Since CA does not have cylinder coordinates, you have to add for each node a force in the corresponding direction. Tedious work. Or you could apply a FORCE_ARRET on the corresponding beams, also tedious work.
You can use the strength of Python to automate this. Depending on the coordinates of the nodes you can apply a force in xy direction. Tedious work, but much nicer.

If this is not the problem you want to solve, pls indicate.

The theoretical solutions: have to see for a solution somewhere: right now I donot have it available (a bit lazy tonight). But be patient, we will come back to this.

So far - kind regards - kees