Extrude To Cylindrical, Curved Body

[fretrip7]

I know there are a number of posts with similar questions, but I haven't been able to find an answer for my situation.  Any help would be appreciated!

I'm trying to create a cavity on the bottom of the guitar neck for the truss rod.  In the model you can see I have a 2D sketch and a 3D sketch and neither will extrude to the curved hollow section inside the neck.  

I've attached my file for review.  My customer is waiting and I am at a road block.  Please help!  Thanks in advance.

[JDMather]

What version of Inventor are you using?

Have you installed all Service Packs and Updates for your version?

Maybe what you want to do is Thicken/Offset surfaces and then Extrude-Cut up to the surfaces

or

maybe what you want to do is Split Face and then Thicken-Cut.

[JDMather]

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@fretrip7 wrote:
... neither will extrude to the curved hollow section inside the neck.  

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Would that curved hollow section completely cap the extrusion, or is Sketch66 microscopically larger then the curved hollow section somewhere along the curve?

[fretrip7]

JD thanks for the quick reply.

I'm using Inventor 2013.  I believe I have all updates.

In regards to the two methods you mentioned, can you please elaborate on the steps?  I'm a little fuzzy with the steps order.

Thanks

[fretrip7]

Sketch 66 is the same width as the tunnel diameter (.25)

Yes, the top of the hollowed section is the stopping point for the cut.

[JDMather]

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@fretrip7 wrote:

Sketch 66 is the same width as the tunnel diameter (.25) 

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I get a slightly  different width, with the 2D sketch slightly wider than the tunnel diameter at at least one location.

Also, go to Help>About Inventor and check your Service Pack.  iProperties seems to indicate that you have not installed any Service Packs or Updates.

If I Offset the slot loop .0001 to the inside to make it smaller - it Extrude-cuts fine.

The problem with the Sweep23 is that you did not create the Sketch63 profile on a plane perpendicular to the start of the Sketch64 path.

But assuming that hole is drilled from the end - you did correctly. 

I would simply use the insignificant offset solution suggested above (cannot measure in real world anyhow).

[JDMather · Accepted solution]

Or even better solution -

Extrude Sketch64 midplane as a Surface and then Extrude-cut to the surface.

Then simply turn off the visibility of the surface body.

[fretrip7]

Perfect! JD thanks a lot for taking the time to answer my question and being so thorough with pictures. You saved my butt! Thanks again.