Extruding ramp on cylinder

[ribblem]

I'm trying to find a way to extrude a ramp on a cylinder.  The method I tried was to extrude a rectangular shape and then use a chamfer.  This is close, but it doesn't do exactly what I want.  The green arrow shows one edge of the ramp points towards the center of the cylinder, which is what I want.  However, the red arrow shows one edge of the chamfer does not.  The second edge is parallel to the first edge and not pointing towards the center of the cylinder like I would like.  I also tried draft and got the same results.

Does anyone have a suggestion on how I could add this kind of ramp feature and have both edges point towards the center of the cylinder?

Thanks for any ideas you can offer!  I'm not an expert in fusion 360 so if you can either explain the technique in some detail or point me somewhere I can learn more about it that would be appreciated.  I just am not sure what to look up to do this.

[g-andresen]

Hi,

please share your design

File > export > save as f3d locally  > attach it to the next post.Please share the file.

günther

[ribblem]

Attached the requested file.

[davebYYPCU]

You cant do as you wish with extrude.

What you are asking for is the face of a coil, 

Simpler to Loft it.  One way to do it.

Might help.....

[ribblem]

Thanks Dave.  I haven't used loft before, but it seemed pretty straight forward.  When I did this it lineally interpolates between profile 1 and profile 2.  The problem with this is this causes it to pull away from the cylinder as shown in the top view image below.

I think this could be solved by using the rails feature in loft, but I'm not sure how to draw a spiral around the edge of the cylinder for this.  Also I'm kind of just guessing at what the rail feature would actually do.

If you can explain how to get a proper loft for this let me know.  I don't see this sort of extra geometry in your example image, but I also can't tell if your example correctly follows the cylinder edge or if it is linearly interpolating between the profiles like mine. If I could control the loft so it only interpolates on the x and y axis, but not the z then I could get it do do what I want, but I don't see that option.

I have attached how I tried to do this.  Thanks!

[ribblem]

I spent some time figuring out how to create a second sketch with projected lines along the edge of the cylinder.  As I thought in my previous post using these as rails fixed the problem there.  However, these rails caused another issue to show up that I don't actually understand why the loft caused if it's doing linear interpolation.  That said I suspect fusion is doing the right thing and my understanding of either the geometry or what loft actually does is wrong.  Anyways I was able to add a second rail to fix that distortion.

I have attached my results.  They are still not quite right.  The ramp feature has is not perpendicular to the part base.  The ramp has a slight twist that I don't really understand.  I have attached the file.  Does anyone know what could fix this or have a suggestion on some other way to do this that isn't as complex as this method is getting pretty involved now.

[davebYYPCU]

I am confused.

Chamfer was not giving a radial top and bottom face edge.

Loft with radial edges as I demo, will not give a planar face, like the chamfer does.

I did not see a correlation of the flat facet faces in the next picture you posted, to the request.

This new file, has original job done, but your not happy.

So because the file name is CAM, are you looking to fillet those radial edges in some way?

Possibly a 3d Spline curve for the ramp face to follow?

[ribblem]

Hi Dave.

I'm having trouble understanding your last post, but I will do my best.  If I get something wrong let me know.

I did not want the chamfer to to be planer in some spots and you are right that the loft is making parts non planer that I want planer.

Maybe the best way to describe what I want is I want the ramp start to be like the loft does, but I want the planes that are close to parallel or perpendicular to the cylinder to be perfectly parallel or perpendicular.

In the image I've attached I added a plane to cut the part to more clearly show the profile of the ramp when using the lofts.  Where that red arrow points, I want a right angle.

I don't need any fillets and I'm not sure what you mean by a spline curve.

At this point I can actually draw exactly what I want in a 3d sketch, but I still don't know of the tools that could be used to transform that into a 3d shape. 

Thanks for all your suggestions so far!

[davebYYPCU]

Ahh, ok, I knew that Loft generates shrinkage, but under estimated how much. Sorry about that.

So a change of tack, the outline of the ramp, your projected rails, are used to cut the inside face with Split Face.  Three ramps 3 Split Face commands.

With that done, it's Offset faces at 6mm to join all together.

Step up my timeline...

I don't like 3d sketches.

Might help....

[davebYYPCU · Accepted solution]

No file, tried again.

[ribblem]

Thanks again Dave.  Your file has a really weird bump, but I found if I extrude 5.99 or 6.01 mm instead of 6.0 it goes away.  There is nothing odd about the model there so I have no idea what is happening and this is the first thing here that might actually be a fusion 360 bug, but I am not very confident in that so I'll probably just ignore it.

I've attached two images.  The first is an offset plane where it looks like the ramp feature is sloped.  However, I realized it was not actually sloped when I used an angled plane to do the cut like you see in the second image.  The strangeness I was seeing was caused by looking at the ramp feature from a skewed perspective.  This was totally my mistake.  Sorry if it caused confusion.

I looked into loft solutions with additional rails and while it improved things I could not get it perfect.  Your solution of splitting the face and then extruding does seem to get the correct answer (except for that one strange issue with 6 mm mentioned above, but I can work around this).  So I will use the split face solution you proposed. 

Thank you.  It's very humbling that I was just thinking I might be graduating from beginner to intermediate with fusion 360, and in this thread I used two new seemingly basic and powerful features of fusion360.  I have lots to learn.  Thanks for all the help!