It does sound like a shell mesh is appropriate for your problem. I guess I'd have to question your comment that the solid mesh is more accurate and reliable though. It might be, for your application, but I have my doubts. My suggestion would be to re-think the way you build your initial geometry. I was at the Ontario COSMOS User Group earlier this week and we discussed this issue at length. If you know a shell mesh is more appropriate for your simulation, consider building surface models with clean edges and intersections so the shell mesh just drops out. Keep the initial model simple with only the detail you need to verify structural aspects. Once you have verified and/or optimized your design, either thicken the surfaces or build your documentation solid from scratch using the lessons learned from the analysis. While appropriate in some cases, using the inside/outside faces of a thin solid model is often very difficult and can result in erroneous results.
While we are working hard to be able to mesh and solve most solid models you throw at COSMOS, there are still significant benefits to using conceptual geometry to get the design right before committing to solids. Every case is different and I'd be happy to take a look at your problem if you want to send it to me but think about alternate workflows to facilitate design innovation and improvement. This is addressed in a couple of COSMOS Companion sessions if you have the time to review these.
Well, in 2009 they REMOVED the possibility to convert solid faces into shell.... now you need to REMAKE THE WHOLE MODEL as surface wuere you need...
You can create surfaces by selecting the face and then Insert->Surface->Offset Surface with a zero value, but it is more work than it use to be.
We use SolidWorks CAD but not CosmosWorks/Simulation. For FEA we use other solver that makes shell models very easily. This is very important when your thickness is smaller than 1/10 of the other two dimensions. Therefore, to be fair with your software and satisfy our client, we would like know more about Simulation 2009 capabilities.
Our customer said to us that:
"Unfortunately I was not able to do any shell meshing because "Solidworks Simulation 2009" automatically determines the optimum mesh. The only way to use shell meshing in "Solidworks Simulation 2009" is the sheet metal feature is used."
1) Cannot he make shell analysis if the model is a solid?
2) How can he perform the shell analysis since it is FEA recommended practice? The thickness is less than 1/10 of the other dimensions.
shell elements need surface geometry to mesh onto. If you don't have a surface just make one from the solid using the offset surface command - then exclude the solid from the analysis or "delete" the solid body (you can always get it back by suppressing the delete feature), ensure you have either bonded contacts or preferably edge consistency (every automatically bonded connection between any two surfaces must share a common edge) to get the connectivities you want. You add a split line to make sure they have a common edge.
One major draw back in 2009 (though not an issue in 2008) is that they restricted the shell definition to surface bodies which is considerably different than an individual surface. While this approach minimizes the work of selecting many surfaces to assign a shell definition, it restricts your ability to apply a doubler by specifying a particular surface as having a different thickness. I frankly haven't done a shell analysis where I ddin't need to do that for a repad or other reinforcemnt. I am sure this was an oversight on SWX's part and I have been told that it is going to be addressed at some point. SWX 2008 is, as far as I am concerend, an extremely efficient tool for building shell models once you get a handle on a productive work flow. I haven't found a more productive package for doing shell models - especially when extracting geometry from solid models. That said though if they improved the splitting (some other FEA tools do this very much better than SWX and I doubt it is a technical challenge), trim, extend and using edge mid points (and offset 1/2 the distance to some other face) in specifying offset surfaces it would be even more productive. I doubt any of this is technically challenging they just don't think very many people want the capabilities. It helps if you make enhancement requests. You can do a high quality analysis with the tool and do it fast but it does take some practice.
Default Default wrote:
I know it takes more time to complete a solid mesh analysis but it gives more accurate and more reliable results compared to the shell mesh.
Thank you Bill!
So, just rephrasing, the customer needs to create surfaces with zero thickness in SolidWorks, suppress the solid parts, specify thickness in Simulation (Cosmos) and treat surfaces as shells.
Is that correct?
Yes, pretty much that's the approach.
All "surfaces" are by definition "zero" thickness.
Depending on within which part the surface that defines the shell lies one could use suppress or delete solid body - if the you put the surface into a different part in an assembly then you could suppress the part that contains the solid. If you put the surface within the same part then you need to use delete solid body.
Just remember - solid bodies line up with solid elements, surfaces (not meaning those associated with a solid) line up with shell elements and to a far more complicated than required degree, lines, line up with beam elements (well at least when using the "structural member" feature and it also works on "extruded geometry" - the lines are inferred from the section centroid and neutral axis or the extruded section. It would be nice if you could just pick a line and make it beam elements but don't hold your breath for that one.). Any connection between element types - ie shell to solids, beam to shell, beam to shell (when it works - some realeses are busted in this respect) and beam to solid must be made with a manually defined connection - bonded or contact and there are rules about how these are made and the result quality you get when you use them.
Thank you again!
Other questions from same customer:
"I was successful at running a simulation using a shell mesh. But I have some questions, because the results do not look convincing. I get large stress concentrations near and around the interface of the lipskin and bulkhead. When I define the thickness of the shell does it treat the surface as the center surface? If so that means I have to offset my surface by half the wall thickness of each component. In simulation, how does it know which direction to apply the thickness? Which surface do I zero offset? I initially assumed to "zero offset" the inner coincident surfaces? (The inner surface of the lipskin and the outer surface of the bulkhead.) Given that assumption, when attempting to define the contact gaps I get a message from the software that there is a gap between the surfaces that might cause some error in my results. The way the surface were created there shouldn't be a gap. If there is a gap and I don't know it, I cannot check it because solidworks cannot detect interference in surfaces. Are my assumption correct, do I ignore the error? "
"I was successful at running a simulation using a shell mesh. But I have some questions, because the results do not look convincing. I get large stress concentrations near and around the interface of the lipskin and bulkhead. When I define the thickness of the shell does it treat the surface as the center surface?
If so that means I have to offset my surface by half the wall thickness of each component.
Well you want to put them in the center but sometime it isn't worth the effort. The rror you introduce on the shell element is typically samll if the distance is large. I would advise running a few test with offset surfaces and ones located at the mid plane. With shells some approaximations of this type are typically inevitable.
In simulation, how does it know which direction to apply the thickness?
It is n't doen within the element it is based on where you put the surface.
Which surface do I zero offset? I initially assumed to "zero offset" the inner coincident surfaces? (The inner surface of the lipskin and the outer surface of the bulkhead.) Given that assumption, when attempting to define the contact gaps I get a message from the software that there is a gap between the surfaces that might cause some error in my results.
If you want to be good and both components are meshed with shell elements extend the the surface to close the gap and split the other surface so they share a coomon edge. Then they will bond with no contact specifications (most of the time - you will see it when it doesn't get it right but this only happens on higher order geometry - sweeps and lofts)
The way the surface were created there shouldn't be a gap. If there is a gap and I don't know it, I cannot check it because solidworks cannot detect interference in surfaces. I use trim and extend and the intersection option inthe split tool.
Are my assumption correct, do I ignore the error? "
The error is a function of the gap and the element size as compared to the shell thickness. Using a bonded condition puts rigid bars between the edge and the other surface - the extent of these bars can make the joint overly stiff or floppy depending on how the software decides to do it. It is best to makethe components share a common edge in shell to shell connections.
Thanks for the directions.
Another question: is it nor easier to make an zero offset surface at internal part to match with another surface considering the external? So both wil be in touch?
Whatever works that makes life easiest is what I do as everything is an approximation. You just need to keep track of how many you are making and what the significance is. A loft of time Just get a nice simple suface to offsett - many time youget a surfce with a very tiny hard to see little notch in the corner. Then to be able to trim and extend easily you need to fill in or cut out the little notch. If you don't have them good on you but if hte solids are thin and depending on how they are nodelled it canbe a pain in the you know where from time to time. I just get a nice simple surface so you avoid the measureing......
i read your conversation and i have a question about shells.
Do you know if i can optimize a shell model?
Some of this may have already been discussed in this post. Here is a summary of some of the steps I use when creating a shell or mixed mesh of an assembly:
- Use symmetry (fixture) when possible (further discussed in help menu)
- If part is not a SM part, create new configuration for FEA. In this configuration, use offset surface (zero or mid-surface) and delete solid body. A shell thickness will need to be defined in the FEA simulation
- In the FEA simulation, create contact set (connections) between sheet metal components that are in contact with each other.
- As h-adaptive meshes (mesh refinement) are not possible for shell meshes, create mesh control in areas of high stress
A shell mesh typically solves faster than a solid mesh due to having fewer equations to solve. The image below is an example of setting-up a shell or mixed mesh in SW2009.