Help with the Sweep Function!

[Boudy25]

Here it is gents i need help with a simple task thats ruining my life. I have two faces of different size and am trying to sweep out a curve section between the two. But since the two faces are of different size it only follows the path with the original face selected. 

[JDMather]

Maybe sweep with guide curve or surface.

Attach the *.ipt file here.

If not Sweep, then Loft.

http://forums.autodesk.com/t5/Inventor-Engineer-to-Order/HELP-Problems-with-Sweep-Function/m-p/47431...

[PaulMunford]

Looks like a candidate for a loft to me. It's difficult to see what your inputs are. Could you upload the part?

[glenn-chun · Accepted solution]

Hi Boudy25,

Loft is more appropriate than sweep in this case since you have two different profiles.  Before you create a loft, add a tangent constraint to your Sketch11 like this:

A loft cut using two profiles and two rails would work.  See "Electric Housing Part 2 (orig plus loft cut).ipt".

I noticed that you used 5 features (3 extrusions and 2 sweeps) when you could create the same shape with a single extrude operation.  I used the following steps in "Electric Housing Part 2 (Glenn).ipt".

1. Extrude a rectangle with a taper angle of -15.25 degrees.

2. Create a loft surface from two profiles and two rails.

3. Remove the material below the loft surface by using the Split tool.

Final result:

Hope this helps,

Glenn

Autodesk ShapeManager Development

[glenn-chun]

Just in case anyone is wondering how I obtained the taper angle from the given taper distance...

tan(theta) = opposite / adjacent
theta = arctan( opposite / adjacent )

tan(taperAngle) = taperDistance / extrudeDistance

taperAngle = arctan( taperDistance / extrudeDistance )
= arctan( 0.3 inch / 1.1 inch )
= 15.2551187 degrees

The minus sign is used for the taper angle since the profile size decreases as it is extruded.

An alternative for the tapered extrusion in this case is a loft between two rectangular profiles.

Glenn
Autodesk ShapeManager Development