I have a pressure vessel which I am trying to analyse. Whenever I convert the solid into 'thin bodies', it loses some of the data. For example, a fillet and a supporting ring (refer to pic attached). I haven't been able to find any 'shell element' settings to adjust.
Also, I need to manually add contacts otherwise the vessel seperates into multiple bodies.
Even though the solid model is in contact, the 'midsurface' shell seperates it. Refer to part file attached.
I briefly tried to run the analysis as a solid model, but gave up as it was taking forever just to mesh.
Thank you for your feedback in advance.
Solved! Go to Solution.
Actually, the Shells behavior you're describing is working 'as-expected'.
The shells work on a per-body basis. To cure the first issue (supporting rings and feet being removed) you can use the multi-solid body approach, so that the supporting rings and base feet are 'new bodies' and not booleaned to the main tank body. Another option is to model it as an assembly and this will be taken care of automatically.
You could choose to keep the rings and feet to be meshed as solid bodies, having a mixed-model simluation (solid and shell element simulation). However, the 'Find Thin bodies' command suggests a using a shell approach for all bodies.
A 'gap' will often be created for a non-constant thickness portion of the model when Midsurfaced. If this is not desired, try using Shell Offset instead of Midsurface. Better yet, adjust the solid model so that it has a constant thickness throughout (such as a typical part with a bend created in the sheet metal environment).
This can easily be done in your model by adjusting the fillet radius in the sketch of the tank for the revolution body. The fillet OD should be ID radius + thickness, or ID = OD - thickness.
I've attached a revised model illustrating these two approaches.
I hope this helps! Please let us know if you have additional questions, comments or suggestions.
Best regards, -Hugh
Oops! Instead of saying " The fillet OD should be ID radius + thickness, or ID = OD - thickness."
It should be " The fillet Outer radius should be Inner radius + thickness, or Inner radius = Outer radius - thickness."
I overlooked the fact that you have to make the circular pattern as 'new bodies' as well.
Apologies for the oversight...
Thank you for your help. That makes sense.
I still had some trouble with the radii missing on 3 of the (patterned) legs. I fixed this by deleting the feature pattern and using pattern in sketch mode.
The pressure vessel also had holes in the bottom where the 3 patterned legs joined to the base. The edit described above fixed this too.
Do you recommend using an assembly over a multibody part? I have found that I need to fiddle around a lot to ensure that all the shell thin bodies keep in contact (selecting midsurface and or offset). If I had it as an assembly, would it automatically keep the constraints and simplify the 'prepare' process?
Can you explain how the 'offset' works? There doesn't appear to be any options for direction/side.
If you can point me to a thin body FEA tutorial, that would be much appreciated.
<<I still had some trouble with the radii missing on 3 of the (patterned) legs. I fixed this by deleting the feature pattern and using pattern in sketch mode.
The pressure vessel also had holes in the bottom where the 3 patterned legs joined to the base. The edit described above fixed this too.>>
Yes, the gaps in the patterned legs were due to not taking the multibody or assembly approach when modeling the legs. The fillets in the legs are constant thickness so they were 'discarded' by the midsurface. The reason for this is that if a face is much smaller % wise. This is done automatically and is part of the midsurface algorithm, it usually doesn't have an adverse effect such as this if the model is prepared with this behavior in mind. I didn't see this effect after I edited the circular pattern using MSB (revised model attached). Perhaps I'm not seeing the effect you're describing in the revised model.
<<Do you recommend using an assembly over a multibody part?>>
Since part and assembly analysis both work on a per-body basis (as opposed to per component-basis) the two approaches are nearly equivalent. The most significant difference is that you can apply different materials in the assembly approach, since we cannot assign a unique material to bodies with MSB's.
A minor difference is in the behavior of feature suppression. In a part analysis, if there are downstream failures of dependent features because it's 'parent' is excluded, those downstream dependent features are excluded automatically. In an assembly analysis, if a dependence such as an (assembly constraint fails due to geometry changes) the exclusion is not possible until this is corrected manually, by adjusting the model accordingly. This doesn't really matter in this model, but is something to keep in mind in case it comes up in the future.
Now that the model is converted to a multi-body model, you can easily use the 'make components' command to convert it to an assembly. I've attached a model taking this approach so you can compare any slight differences in behavior
<<I have found that I need to fiddle around a lot to ensure that all the shell thin bodies keep in contact (selecting midsurface and or offset).>>
I cannot see this effect in the simulation, but I may be missing something.
<< If I had it as an assembly, would it automatically keep the constraints and simplify the 'prepare' process?>>
Assembly constraints are not taken into account in the contact type generated automatically generated (i.e. all are created as Bonded by default) if you need to adjust the contact type, you can manually edit the automatic bonded contact(s) and change them to say Separation if needed.
<<Can you explain how the 'offset' works? There doesn't appear to be any options for direction/side.>>
The Wikihelp briefly describes the dialog functionality here. The Offset works the same as the Thicken / Offset modeling command for creating an Offset surface. The reason we can only offset in one direction is because we want to put the offset shell surface 'inside' the solid model. The direction can be changed indirectly by choosing the 'inside' versus 'outside' face.
To illustrate how offset works graphically, looking at the side profile of a cross-section of flat plate:
<<If you can point me to a thin body FEA tutorial, that would be much appreciated.>>
Unfortunately, there isn't a Stress Analysis tutorial dealing with Shells that I can find.
We appreciate your feedback. Please let us know if you have additional questions, comments or suggestions.
Best regards, -Hugh
[Edit: Added comment about 'inside' versus 'outside' face and added attachments]
This sounds like it falls under the class of a thin wall vessel? I'm not familiar with Inventor's FEA capabilities. But I have experience performing FEA on pressure vessels created in Inventor. In the past, what I've done is create a surface model of the vessel in Inventor. Imported the surface model into the FEA software and it worked fine. If your designing per ASME pressure vessel code, and it is a thin wall vessel, typically only Membrane stresses (hoop stress and longitudinal stress) with different load conditions are needed. The surface model will yield these results. Then, and you may already do this, its good practice to validate the model with some hand calculations.
Log into access your profile, ask and answer questions, share ideas and more. Haven't signed up yet? Register
Start with some of our most frequented solutions to get help installing your software.