Q) Can gasket elements be defined in WB Simulation?
A) Although in the current release of WB Simulation (as of this writing, it is version 11.0) there is no direct way to add gasket elements, this can be done easily with a Commands object. Postprocessing of gasket output quantities would need to be done with an additional Commands object under the "Solution" branch or done interactively in the ANSYS General Postprocessor.
Note that gasket elements require special node numbering to define the 'bottom' and 'top' faces, as the pressure-closure relationship is essentially a 1D constitutive model defining the stiffness behavior in the through-thickness direction.
One can take advantage of the fact that WB Simulation has a sweep meshing capability for SOLSH190 in 3D, as the SOLSH190 and INTER195 numbering are identical. This allows the user to correctly define the orientation of the through-thickness direction for gasket elements, regardless of how the geometry is oriented.
Also, if higher-order gasket elements are used, note that INTER194 and INTER193 do not have midside nodes along the thickness direction, so special attention is required for those cases.
To add 3D, lower-order gasket elements (INTER195):
1) Add a "Mesh branch > Method" object for the gasket part. Ensure that "Method: Sweep" and "Src/Trg Selection: Automatic/Manual Thin Model" are set.
2) Under "Geometry branch > Part(s)" of the gasket parts, insert a "Commands" object with the following contents:
---begin
ET,matid,null
ET,matid,195
MPDELE,ALL,matid
TB,GASKET,matid <...>
TBDATA <...>
---end
The actual gasket material parameters in "<...>" need to be specified by the user.
3) Connect the gasket part to other parts via bonded contact, if they are not a multibody part.
This will allow that part to be meshed with INTER195 elements as well as have user-defined gasket properties.
As noted above, gasket postprocessing would be done interactively in ANSYS or by inserting the relevant comma
|
Q) Can gasket elements be defined in WB Simulation? A) Although in the current release of WB Simulation (as of this writing, it is version 11.0) there is no direct way to add gasket elements, this can be done easily with a Commands object. Postprocessing of gasket output quantities would need to be done with an additional Commands object under the "Solution" branch or done interactively in the ANSYS General Postprocessor. Note that gasket elements require special node numbering to define the 'bottom' and 'top' faces, as the pressure-closure relationship is essentially a 1D constitutive model defining the stiffness behavior in the through-thickness direction. One can take advantage of the fact that WB Simulation has a sweep meshing capability for SOLSH190 in 3D, as the SOLSH190 and INTER195 numbering are identical. This allows the user to correctly define the orientation of the through-thickness direction for gasket elements, regardless of how the geometry is oriented. Also, if higher-order gasket elements are used, note that INTER194 and INTER193 do not have midside nodes along the thickness direction, so special attention is required for those cases. To add 3D, lower-order gasket elements (INTER195): 1) Add a "Mesh branch > Method" object for the gasket part. Ensure that "Method: Sweep" and "Src/Trg Selection: Automatic/Manual Thin Model" are set. 2) Under "Geometry branch > Part(s)" of the gasket parts, insert a "Commands" object with the following contents: ---begin ET,matid,null ET,matid,195 MPDELE,ALL,matid TB,GASKET,matid <...> TBDATA <...> ---end The actual gasket material parameters in "<...>" need to be specified by the user. 3) Connect the gasket part to other parts via bonded contact, if they are not a multibody part. This will allow that part to be meshed with INTER195 elements as well as have user-defined gasket properties. As noted above, gasket postprocessing would be done interactively in ANSYS or by inserting the relevant commands under the "Solution" branch. Please refer to the ANSYS 11.0 help system for details on INTER195 (Elements Reference), gasket material (TB section of Commands Reference), as well as general procedure/information (Chapter 10 of the Structural Analysis Guide). |
||
|