How to extrude/emboss circular pattern/text on Cone shape?

[coryjamesmillercl]

I am a beginner with Fusion outside of simple objects, so if this is easy and I have missed it I apologize.  I am trying to recreate a know that has a skirt (see image).  Around the image there are markings, numbers, text, and a circle.  I would like to add this and emboss or recess it into the skirt, so that after I print it I can add paint in the recessed/embossed area.

Where do I start?  I was able to project a couple of circles onto the skirt, but then couldn't figure out how to actually extrude/recess the area.  Is that the idea though?  Draw everything out on a 2d sketch and then project onto the skirt face?

I did see a bunch of videos on adding text to a cone (essentially my skirt) but in this case the markings/text need to be equally spaced, etc....so I wasn't sure if it would 100% correlate.  Same with videos on adding features to a cone (https://www.youtube.com/watch?v=Z_imovRajhc).  I thought maybe the individual markings could be done this way, but wasn't having much luck after projecting to the surface.

Any help or guidance is appreciated.

[etfrench]

Start with a sketch on the XZ or YZ origin plane.  Draw a rectangle the height of the tallest line. Draw another line horizontally at the midpoint of the rectangle.  Draw another line halfway between that and the bottom.  Deboss the bottom quarter profile.  Circular pattern it 100 times.  Deboss the bottom half profile.  Circular pattern that 20 times. Deboss the full profile.  Circular pattern that 10 times.

If you want to 3d print this, create a copy (paste new) of the knob, then combine cut the original from the copy with keep tools enabled.  This will give you the separate bodies for printing in a different color.  The horizontal line can be simply revolved.  The text can be embossed from separate sketches.

p.s. You can use the Suppress option in the circular patterns to remove the duplicate bodies.

[TheCADWhisperer]

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@coryjamesmillercl wrote:

I am a beginner with Fusion 
Any help or guidance is appreciated.

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@coryjamesmillercl 

Would you be willing to start over from scratch with step-by-step instructions on how to model this correctly?

[coryjamesmillercl]

@TheCADWhisperer if there is a better way to model this I have no issues starting over.

[TheCADWhisperer]

@coryjamesmillercl 

OK, let's get started. (I am going away for a couple of days and not sure how much internet access I will have so stick with me on this.)

Obviously, this isn't going to work...

And you should never have a sketch of this complexity - so we will fix that...

[TheCADWhisperer]

@coryjamesmillercl 

Step 1. 

Create this sketch exactly as shown (note the Centerline vertical from the Origin.)

Attach your progress here for next step.

[coryjamesmillercl]

@TheCADWhisperer I wasn't sure exactly how to 'attach the sketch'.  So here's a picture and also exported file.  If there is better way to post it let me know.  I also had created parameters for a bunch of the measurements in case I wanted to change later.

[TheCADWhisperer]

@coryjamesmillercl 

Good job on the sketch.

Now do a Revolve and then Shell... 

(If you don't really want Shell, just do it my way to start and then you can change later.)

[TheCADWhisperer]

@coryjamesmillercl 

Now Edit Sketch1 and add these two vertical lines.

Finish Sketch1.

Make the sketch visible again and Revolve-Join...

[coryjamesmillercl]

@TheCADWhisperer Thanks again for stepping me through this.  Here's my latest updates.

[TheCADWhisperer]

@coryjamesmillercl 

Edit Sketch1: Add this third vertical line. Dimension from the Origin (not the centerline).

Now Extrude this rectangular profile as Join,

I just eyeballed the .25 dimension to be "far enough" but would rather set as a parameter incase dimensions change.

In the next few steps we get to the fun stuff.

[coryjamesmillercl]

@TheCADWhisperer Done.

[TheCADWhisperer]

@coryjamesmillercl 

Edit Sketch1 and add these two lines...

Extrude - Cut symmetrically as shown...

Circular Pattern the feature...

[TheCADWhisperer]

@coryjamesmillercl 

Add two more lines.

Make the longer lines =

Extrude - Cut...

Circular Pattern 20 times.

You know where we are going next...

[coryjamesmillercl]

@TheCADWhisperer Done.

[TheCADWhisperer]

@coryjamesmillercl 

Start a New Sketch on the YZ Plane (parallel to the flat in the hole).

Now p for Project and select the centerline and then create a Sketch Point on the Centerline as shown (be careful to NOT click on the midpoint of the Centerline unless that is where you want the Tapped Hole).

Now create the tapped hole, but do not set to Modeled just yet.

[coryjamesmillercl]

@TheCADWhisperer I believe I'm caught up now.

[TheCADWhisperer]

@coryjamesmillercl 

I didn't explain why we put the rectangle for the straight knurl at the midpoint.

If we had put it tangent to the cylinder it would only touch along that line after extruding.

We had to embed by some nominal amount - midpoint is easy and logical.

[coryjamesmillercl]

@TheCADWhisperer Threaded hole has been added.