'Error: Inconsistent face' when trying to split a body

[lure23]

I've imported a model made in Rhinoceros and since it's symmetrical I thought to reduce complexities and use mirroring.

There are no straight lines in the model so I ended up pulling an offset plane to what seems to be the mid point and using 'Modify > Split Body' to cut the cabin in half.

This did not work. Here I've applied it only on one body, and show the resulting error message. 

Any idea what's wrong with the model and can I do something to chainsaw it in two, delete the left half and use 'mirror' to re-create from the right half.

Thanks.

Addendum.

I may be into something. 

I can split the remaining pieces by the 'Modify > Split Face' tool. Which raises some questions:

1. Why should there need to be separate 'Split Body' and 'Split Face' tools?

2. Why are the faces being split listed as 'Body13' (etc.) in the Browser? 

Using 'Face' in the Browser would be consistent.

[innovatenate]

Asko,

Any chance you could share the model with me? I believe I still have access to a few files in one of your groups.

Kind Regard,

[AndrewSears]

Asko,

Have you solved this?  Is it possible to share the file or add us to your group?  If so, send group invite to andrew.sears@autodesk.com.

Andy 

[innovatenate]

Hi Asko,

To clarify the 'Body' nomenclature, there are two types, surface bodies and solid bodies. In the Fusion 360 browser, they are all denoted as bodies, but there is a difference. One similarity are a collection of faces, edges, and wires. To call a surface body a face would be inaccurate since they can contain multiple faces and other geometries that are "stitched" together to form a single surface body. The major difference between solid bodies and surface bodies is that a solid will fill the interior volume of the faces, edges and wires if the volume is "water tight." I should note that the Patch environment in Inventor is very useful for converting surface bodies into solid bodies, should you ever find the need. You can create patch surface, merge faces together and finally, stitch everything together.

The reason there is a split face and split body command is that sometimes you need to only split a face on a solid/surface body and not the entire "body." This can be especially helpful for simulation (i.e.. providing a face to place load/constraint condition). In fusion, you may only want to push/pull on part of a face. I can elaborate further on this with an example if you'd like, just let me know.

I have a suggestion for getting the precise symmetry plane if there's not other geometry around to create an offset construction plane from. 

Procedure

1. Create a sketch and use the project feature to project two points that should be equidistant from the centerline of the pod.

2. Connect these two projected sketch points with a sketch line

3. Add another perpendicular line that utilize a midpoint constraint (triangle symbol) to split the pod

4. Extrude this line into a surface plane that can be used to split the body. 

See the screenshot below for clarification.

As for splitting Body 13, I found that I was able to use the split body command after using the Patch > Modify > Stitch command on Body 13. I'm not sure exactly what the error message was indicating, but I will submit a user experience report to development based on this thread. I've uploaded a sample file to your hub for your review. If you have any difficulty locating or accessing it, please let me know.

Let me know if this helps or if there are any points I've missed, questions or concerns, etc...

Kind Regards,

[lure23]

Thanks, Nate for a very fine clarification.

I had thought of ”body” as in ”body mass” (meaning it would always have a volume).

Maybe ”surface” would be sufficient term for the surfaces = 1..n faces, no volume.

Going alongside that, ”solid” would be enough for solid bodies.