Dovetail Groove swept along a curved surface

[AWACS963]

Hello all, as you can tell I am new here to the forum and only recently started using Inventor again after a 13 year "vacation" with Unigrpahics (NX7). Anyway as the Subject line indicates I am having issues creating  an o-ring groove along a curved surface. I projected the profile on to my curved surface followed by a successfull sweep. I then had to use  "sculpt" to subtract  the swept feature from my main body. This was all striaghtforward but what I need is for the  swept profile to orient itself normal to the surface  along the entire path. Which is not happening. ANy suggestions would be wonderful.Thanks in advance

[CCarreiras]

Hi!

Like in NX7, you have to give additional information if you don't want a "pure Sweep".

For your case, choose the cylinder surface to give an alternative orientation to the sweep.

Select "Path & Guide surface" and pick the cylinder surface, and that's it.

(Also constrain the sketches and turn geometry unnecessary to profile as "work geometry", but i know, this was only a test)

Did you find this reply helpful ? If so, use the    Accept as Solution or Kudos - Thank you!

[JDMather]

In addition to the information provided - you have some extraneous geometry in Sketch1, including a zero length line - I imagine this would not be good in any CAD program.

As you gain experience you will discover that the Work Plane1 and ExtrusionSrf1 are not needed to model this part.

Also, if you use a centerline type in Sketch1 - you can dimension the diametral dimensions.

and,

there are two Service Packs available for 2014.

[JDMather]

Notice that extruding the surface projects directly onto the cylindrical face resulting in 3D sketch intersection not equal distant from cut.

I suspect your true design intent is to have this equal distance, correct?

Open the attached file and edit Sketch1 and examine.  Compare and contrast to your sketch.

Edit Sketch2 and examine.  Compare and contrast to your sketch.

Does Sweep look OK?

Drag the red End of Part marker in the feature tree below Extrusion2.

Now examine the groove from end view.

This type of geometry requires another trick.

[AWACS963]

First off thanks all for the help.

 Couple of things; when you pick your path for the sweep are you simply picking the slot shaped edge fomed by extrusion 1? Secondly ,yes I do need the  dove tail groove equidistant from the "slot shaped edge" but equally important I need the orientation of the groove normal to the surface which it is not. see below. The purpose if not obvious is to insert an o-ring into this formed dovetail groove