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.
Solved! Go to Solution.
Solved by glenn-chun. Go to Solution.
Maybe sweep with guide curve or surface.
Attach the *.ipt file here.
If not Sweep, then Loft.
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
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