Fusion 360 emboss shape on cylinder with draft

[lstam16]

Hello!
Check my attached images please.

attached image "Desired pattern" is my aim.

Following Problem:
When The surface is getting angled I can not project my desired pattern to it anymore without that it warps/rotate weirdly.

I have attached some tryouts.
Please explain it to me how to do it or do it yourself.

I have tried the following methods (without success):
- Sketch + Emboss
- Sketch + Extrude + split surface + remove outer body + pull/extrude inner body.

This is urgent!
Please hit me up asap.

[jhackney1972]

If it is urgent, then attaching of your model, containing the sketch you want, would speed things along.  If you do not know how to attach your Fusion 360 model follow these easy steps. Open the model in Fusion 360, select the File menu, then Export and save as a F3D or F3Z file to your hard drive. Then use the Attachments section, of a forum post, to attach it.

[jhackney1972]

You did not attach your model so I quickly threw together a model to illustrate an alternative method of achieving your emboss on a tapered cylinder.  You can vary the depth of the pattern by changing the Surface offset, third item from the right, in the timeline.  Model is attached

[etfrench]

Here's one method:

1. Create a helix in the Surface workspace using a sweep with a horizontal line for the profile, a vertical line for the path, and a 60 degree taper.
2. Use that to Split body a cone representing the extruded diamond thickness.
3. In the Surface workspace offset the side face of the split body the desired width of the sides of the diamonds.
4. Use that to Split body again.
5. Remove or hide all of the excess bodies.
6. Mirror the side of the diamond. (join the mirrored body to the original.)
7. Circular pattern that body (Any 6 copies will form a diamond).
8. Revolve the inner cone.

p.s. The taper angle of the helix can be any angle which can divide 360 degrees evenly (except for 180).

[etfrench]

If you want nice pointy ends on the top, you can use the offset face command in the Surface workspace.  After extending the offset, Press pull the top of one side of a diamond through the offset. Split body to remove the excess.  Repeat for the other side.