Q: A user has a surface model of a cylinder. (i.e., A common pressure vessel.). If you apply a frictionless support to the symmetrical edges, the results do not appear correct.
How can I correctly apply a symmetry boundary condition to a surface model?
A. Applying a frictionless support to the symmetrical edges are not correct for a surface model. This will only work for Solid models..
Shell models have rotational degrees of freedom, which must be accounted for.
Workaround
1. Create a Named Selection scoped to the cut edges of the symmetry plane. Name it "cut_edge".
2. Insert a Commands Object using the following
! Commands inserted into this file will be executed just prior to the Ansys SOLVE command.
! These commands may supercede command settings set by Workbench.
! Active UNIT system in Workbench when this object was created: U.S. Customary (in, lbm, lbf, F, s)
cmsel,s,cut_edge,node
d,all,rotx,0
d,all,roty,0
d,all,uz,0
cmsel,all,all
3. The best explanation of how to apply symmetric boundary conditions is in the Ansys Basic Analysis Guide, Section 2.6.4., Applying Symmetry or Antisymmetry Boundary Conditions
4. Simulation V10.0 will have a Beta feature that will allow you to insert a "Symmetry Condition" into the Model Branch that will automatically handle the application of BC's for symmetry.
|
Q: A user has a surface model of a cylinder. (i.e., A common pressure vessel.). If you apply a frictionless support to the symmetrical edges, the results do not appear correct. How can I correctly apply a symmetry boundary condition to a surface model? A. Applying a frictionless support to the symmetrical edges are not correct for a surface model. This will only work for Solid models.. Shell models have rotational degrees of freedom, which must be accounted for. Workaround 1. Create a Named Selection scoped to the cut edges of the symmetry plane. Name it "cut_edge". 2. Insert a Commands Object using the following ! Commands inserted into this file will be executed just prior to the Ansys SOLVE command. ! These commands may supercede command settings set by Workbench. ! Active UNIT system in Workbench when this object was created: U.S. Customary (in, lbm, lbf, F, s) cmsel,s,cut_edge,node d,all,rotx,0 d,all,roty,0 d,all,uz,0 cmsel,all,all 3. The best explanation of how to apply symmetric boundary conditions is in the Ansys Basic Analysis Guide, Section 2.6.4., Applying Symmetry or Antisymmetry Boundary Conditions 4. Simulation V10.0 will have a Beta feature that will allow you to insert a "Symmetry Condition" into the Model Branch that will automatically handle the application of BC's for symmetry. |
||
|