Cannot split body made with loft and shell

[Anonymous]

I have a problem that I have been trying for days to get around. 

I am building a model airplane fuselage (to be 3D printed) and I have created a body using loft and then shell. I have also added a few internal features inside the hollowed out body.

Now I want to use a surface to split the body into two parts, the fuselage and a canopy. However, I get the error message:

"Create parting line failed Flygplanskropp sliced150424-1.ipt: Errors occurred during update Split1: Could not build this Split Split feature could not create two bodies. Change the Split Tool so that split feature can create two bodies"

It does not seem to matter which surface I use, I have tried with different work planes.

Having tried a number of different things I have seen that if I suppress the "shell" command then the split will work, but this will not help me...

I am stumped, I really cannot figure out what I am doing wrong and I have not found any other posts with a solution. 

Thanks for any help!

[JDMather · Accepted solution]

The problem seems to arise with FireWall extrusion.

Do the Splits before that feature.

(drag the red End of Part marker above that feature, add you geometry to do the splits and split the part)

(you don't need the extruded surface to split the part - only a sketch)

You might need to recreate the Firewall and Motor Mount holes last.

Also, you should install the Service Packs and Updates for your version of Inventor.

[Anonymous]

Fantastic! Thank you very much! 

Still have no idea why the firewall extrusion caused problem, I suspect is has something to do with it being based on projected edges. Anyway, it is easy to fix like you suggest. Installing the service pack sounds like a good idea. 

May I ask how you found out that it was the firewall extrusion that was the problem? 

 Again, thank you.

[JDMather]

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@Anonymous wrote:

...

May I ask how you found out that it was the firewall extrusion that was the problem? 

 Again, thank you.

I rolled up the EOP and tried Split at each feature till I found where it failed.

[Anonymous]

Thanks, I will try that next time I run into problems.

I think I found the problem with the "firewall" extrusion; it was extruded in the direction where the "fuselage" was expanding, like a funnel. This means that the firewall extrusion was not properly attached to the fuselage since the extrusion is cylindrical, see picture below. When I extruded in the other direction it works fine.