I have a model which is meshed using 3D hex elements in which surface-to-surface glue constraints are being used to constrain the bodies together and the simulation process also requires creating a very thin surface coat of 2D elements on top of some of the 3D elements. Because there will probably be part updates (using jt files) I would like to use Geometry mode to define the surface coat elements and not use MMCs to connect the bodies.
This means that the faces that are used to create the simulation regions for the glue constraints are associated to both the 2D surface coat elements and the 3D element faces. And when the solver file is written it uses the 2D elements and creates a BSURF card when I want the glue constraint to be applied to the 3D element faces using a BSURFS card.
Is there a method available to have a region ignore any 2D elements associated with the polygon face?
I've sent a message to development regarding this question, but I suspect there is no way to force the use of the solid element faces when the face has solids and shells on it. I recall conversations over the years regarding contact/glue regions on this topic. Our conclusion was that the shell is the outermost entity on the solid, so why would you ever NOT want to use it? In this case maybe the shell thickness is what you want to eliminate from the contact calculations. If so, then you could define a negative offset on the contact regions equal to half the shell thickness. That would place the contact region back onto the solid face.
I'll send out another reply if development responds positively to being able to force the use of the solid element faces.
Simulation Product Management
Product Engineering Software
Siemens Industry Sector
Siemens Product Lifecycle Management Software Inc.
I would assume that the shells are thinner than the solid that they surface coat. If this is a membrane coating, they would be much thinner. In that case, the thickness offset (which can be easily disabled on BCTPARM) is much less of a concern than the auto calculated contact stiffness. The calculated contact stiffness for the shells would be less (much less for membrane coating) than if it was calculated for the underlying solids. This could lead to convergence problems or bad contact results.
If the contact stiffness is entered manually (via PENN/PENT on BCTPARM), then it really does not matter if the region is comprised of the shells or the underlying solid faces.
Thanks for the reply and what you are describing is what I am seeing, when the surface region uses the shells the stiffness between the bodies is much less then if the surface region used the solid element faces. But I am not using the regions to define surface-to-surface contact objects but surface-to-surface gluing objects (weld like). So I need to use the solid element faces for the regions in order to have the bodies remain glued together. If the region uses the shell elements then the bodies move away from each other.
Sorry. For glue (to the shell coating), you can try the following:
You could make a run where you manually define glue to the solids and see what the auto calculated PENGLUE value is. Then specify that value in subsequent runs where glue is defined on the shells.
Thanks for the reply. The reason why we don't want to use the shells to glue the bodies together is that they are only there for post-processing reasons, they do not represent an actual component in the system. The output requests for the simulation only requests stresses/strains for the shells and not for the solids. This can significantly reduce the size of the .op2 file for even a small model but particularly for a large model (not to mention the reduction potential depending on the number of normal modes computed) and reduces the amount of time it takes to post process the results.
If we used Free Coincident MMCs to connect the bodies then faces would be etched into the polygon bodies in the FEM and we would not create 2D surface coat elements on the faces that would be used for the glue constraints. But then it would be more time consuming to update the FEM and SIM after any CAD geometry updates.
Those reasons make sense to me. I think Jim's got the best solution for you.
There is another option that involves multiple steps and deck editing to get an input file for the solve. You can edit the shell mesh associated data to NOT export the meshes. Then in the SIM, the shell meshes don't exist. The glue is forced to use the solid faces. Write out an input file without the shells. Then edit the shell mesh associated data to export them. You can selectively export just the shell elements (File, export, Simulation) and include that file with the solution's input file.
Alternatively you could selectively export or preview the glue simulation object and include that in a model that doesn't include glue, but does include the shells. Include the glue file in the solution's input file and edit the case control to account for the glue.
Since I'm into deck editing, I'm sure there are other ways to get to what you need. These are all the ideas that we came up with after running your question through development.
Mark & Jim,
Thanks for the ideas. Because all the solutions will require manual changes to FEM or SIM components after a CAD part update we may have to try several and see which requires the least work. We did find another method which is to use the Element Face mode when creating the surface coat elements. This does not associate the shell elements to the polygon faces so the Regions in the SIM file will use the solid element faces and create a BSURFS card. Of course this means that the following steps will have to be followed for any CAD geometry updates:
I'll talk with our support team here about getting an Enhancement Request turned in to allow the user to specify ignoring surface coat elements in Region definitions.