How to convert a solid model to surfaces

[John_Holtz]

Hi everyone,

As you may know, Inventor Nastran can convert a solid model to shell elements. This is done with the "Prepare > Find This Bodies" or "Prepare > Midsurfaces" command in the Nastran environment. This approach may not be the best method for some situations, as follows:

• When the number of midsurfaces (and corresponding idealizations) becomes large, Inventor Nastran can become slow. (Takes a longer time to enter the Nastran environment, etc.) 
• Since midsurfaces are created at the midplane of the solid, adjoining surfaces are offset by some distance. "Contacts > Solver" makes it easy to compensate for this, but contact introduces an approximation and may not be suitable for some models. Continuous Meshing that creates a matching mesh between adjoining faces is a better solution but requires the faces to be touching. (Thermal stress is one example where contact creates an issue since the contact prevents expansion at the joint between bodies.)

Since building the model only happens once and using the model in Nastran often occurs many times, it is better to spend a little more time in Inventor to create a surface model than to wait multiple times in Inventor. (At least, I generally need to run a model multiple times to work out my mistakes. Maybe other people get it to work on 1 try: 1 and done as they say. 😁) One way to avoid the above issues is to create a surface model in Inventor. Since "everyone" has a solid model and "no one" creates a surface model from scratch in Inventor, it would be nice to be able to convert the solid to a surface in the Inventor modeling environment. Here is one approach that can be used. See the attached files:

• "How to convert a solid model to a surface model using Inventor.docx" describes the process. I will add the basic steps below for those who are experienced with Inventor modeling.
• "Convert solid to surface.mp4" is a video showing the process on the sample model.
• "Example model.zip" includes two samples (created in Inventor 2022, so useable for 2022 and newer versions). "single part solid to shell.ipt" is the original solid model that gets converted to surfaces, and "Assembly from single part.iam" is the final model that is used in Inventor Nastran.

The basic steps for converting the solid CAD model to a surface CAD model are as follows:

1. Offset the faces using “3D Model > Modify > Thicken/Offset”. Offset them by 1/2 the thickness.
2. Use "3D Model > Surface > Extend" as desired so that the adjoining surfaces actually touch. (Likewise, use "3D Model > Surface > Trim" to cut off any portions that overlap.)
3. Split surfaces using “3D Model > Modify > Split” to create smaller faces to apply loads or to create more edges to improve continuous meshing in Nastran. (This step is not detailed in the document or in the video. I did not think of it until after I was done!)
4. Put surfaces of the same thickness into a part file using “Manage > Layout > Make Part” which simultaneously creates an assembly. (This is optional but makes it much easier to define the idealizations in Nastran.)
5. Enter Nastran and define the Idealizations. By hiding parts and use a rectangle selection, all the faces that have the same shell thickness can be easily selected.

If any Inventor modeling experts have other suggestions, please feel free to add your thoughts.

John

[ecottingham3KD7X]

In this example the solid model is a part file that has been created with extrusions illustrating a plate sitting on H beams.

For an assembly consisting of plates with wide flanges and channels how would you surface the parts and assembly? 

Thx