ramp down in circle

[Outpost31d]

Hello I am a bit stuck on my simple design.  I am trying to create a ramp from the top piece to the bottom piece to follow the curvature of the circle, as indicated in my design below. To recreate the photo of the piece below that.  Just wondering if anyone had any suggestions on the best way to do that? https://a360.co/2vn31UR

[davebYYPCU]

Not sure of the underside of the ramp, but best guess.

Step up the timeline...

Might help....

[davebYYPCU]

After posting the previous message, I went on to pattern the ramp, and it doesn't fit, would not combine.

The sketches are not well constructed, you have used mirror, but the lug was not radially aligned.  

Can't fix it, have no idea which tooth was the original.  

Blue sketch lines should keep you awake at night.

[TheCADWhisperer]

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@Outpost31d wrote:

Hello I am a bit stuck on my simple design. 

What is the reason that you are modeling this part?

There is nothing simple about gear design.

Almost everything you have done is incorrect.

Even your circles are unconstrained.  This is the simple part of the design.

You should model only one tooth and pattern body rather than sketch elements.

Your gear tooth profile is incorrect.

The helical ramp would take an advanced understanding of modeling techniques.

Have you completed any simpler designs before this one where you gained experience in fully defining sketches?

[chrisplyler · Accepted solution]

Meh...

The only thing a helical ramp takes an advanced understanding of is using the Sweep tool with a Twist Angle. There are, of course, other ways of doing it. But for the OP's desired geometry, I think this is the easiest way.

https://knowledge.autodesk.com/community/screencast/00c75e99-291f-4d8e-a8f3-c70ee4b4ec46

[TheCADWhisperer]

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@chrisplyler wrote:

The only thing a helical ramp takes an advanced understanding of is using the Sweep tool with a Twist Angle.

 Let's take it to manufacturing (in the real world, not Fusion manufacturing) and also assemble your mating part.

[chrisplyler]

I don't have a mating part. The OP didn't specify anything about a mating part. It's not my fault if my technique isn't suitable for a condition that wasn't mentioned.

[Outpost31d]

Thanks for your help, appreciate it!  I will work on my sketches.  I found chrisplyler's suggestion worked well for my application.  I can now sleep at night 🙂  redone here https://a360.co/2vn31UR 

I have much to learn.

[Outpost31d]

Thanks so much! Your video explains it perfectly.  That technique worked really well.  Appreciate your time on this.  I redid it here https://a360.co/2vn31UR 

[Outpost31d]

 The reason I am modeling this part is for a lawnmower engine starter.  I did not mean to offend anyone by stating that gears are simple so sry about that.  I constrained my circle as you suggested and modeled one tooth and patterned that body as well, just curious why do that instead of from the sketch?  Chrisplyler's video worked quite well for the helical ramp.   I am new to CAD so this is certainly a challenge for me.  Hopefully I can move away from doing everything wrong at some point : )   Here is what I came up with, https://a360.co/2vn31UR  please feel free to point out anything else you think I could improve on, thnx!

[davebYYPCU]

Your ramp is backwards to the first one.

Not many black lines in the first and last sketch.

Do you see the blue snap cursor indicator when drafting?  Your concentric circle / arcs are not snapped to the origin, and as soon as you fix that a lot of the sketch turns black.

Sketch lines colours, have meaning -

purple and black fully locked, (ideal)

green fixed (should be avoided)

blue and orange not locked, (can be dragged out of position, - should keep you awake at night).

What I would do is highlighted, after snapping the circles to the origin. 

Move the tooth to align with the lug, and you only have one mirror line.

Might help.

[chrisplyler]

Patterns in the model workspace (faces, bodies, features, etc.) are preferable to patterns in the sketch workspace as a general rule, although there are exceptions you might discover if you model regularly wherein a certain desired result just isn't possible unless you do it in the sketch.

One good reason for this is sketch simplicity. Overly complicated and/or crowded sketches seem to bog Fusion down, because it's more math solving that has to be done, ESPECIALLY if they aren't constrained well. Depending on how crowded they get, it's also just a nuisance to work in them. Another reason I've found is that it's much easier to edit the pattern after the fact if you've done it in the model space, because it gives you an event/feature in the timeline. There are probably other reasons too, but those are my personal biggies.

Same thing applies with fillets and chamfers. If you can, the sketch the primary shape, then add fillets and chamfers as modeling events/features at the end.

[Outpost31d]

Ok got it, I will give your example a try tonight, thanks so much! 

[Outpost31d]

Thanks for the explanation, now I see why it's important, defiantly something I need to do!