A constraint problem with intersecting circles

[Anonymous]

I have been working with CAD and Fusion 360 for about 3 weeks, and have been trying for few days to figure out why I can't extrude the outside part shown on the attached screenshot. The points at the intersection of the two circles are constrained as Coincident. All I'm trying to do is have a circular groove on a larger circle within a rectangle. Please help.

[Anonymous]

Can you share your file to check it out?

Gilmer J. Vizconde

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If it was useful please mark as a solution and give me kudos  

[davebYYPCU]

Your pic shows you have the inside profile selected, with the sketch in edit mode.

Stop the sketch, then select the other profile, to extrude it.

Like this...

[Anonymous]

Thanks for looking at the attached design. I created a simplified version to minimize your dealing with my parameters up to the problem issue.

[Anonymous]

Thanks for your consideration. Your example shows what I'm after, but It doesn't work for me in either Sketch mode or not. It shows red lines and Extrude refuses to work. Did you fool around with constraints to create your example?

[jeff_strater]

Hi @Anonymous,

I tried this with the design you shared (thanks for sharing the design).  It seems to work OK, see the screencast.  Is this what you were trying to achieve?

BTW, it shouldn't matter what the constraints/parameters are here, you should be able to just select the profiles you need inside of the Extrude command, enter a distance or drag the arrow, and the Extrude should work fine.

Jeff

[Anonymous]

Thanks to those checking this out for me. Unfortunately I failed to included the apparently most important facts that along with the extrude I am using a positive taper as well as a negative extrude length to keep the face on the top. I have no problem without the taper.

[jeff_strater · Accepted solution]

The taper is the problem.  Actually, the combination of distance and taper will eventually produce an invalid, degenerate body.  At a distance of -10mm, I can only add 4.28 degrees of taper before the small channel becomes degenerate.  So, less distance, or less taper will result in success:

Jeff

[Anonymous]

Thanks for  very clear explanation. It appeared that to achieve my goal I needed to maintain a constant arc angle instead of the small circle so I tried using a 3 point arc, but it  still won't let me Extrude beyond a few units. Any ideas will be appreciated.

[TheCADWhisperer]

Do you have a picture or link to something similar to what you are trying to design.

I suspect the solution is very easy.

[Anonymous]

Hello  @Anonymous

To achieve that.

At first make the extrude and taper with only de circle inside.

Then do the next operation, make a extrude cut only with the constant arc across the body and voila.

Let me know if you were looking for that.

 https://screencast.autodesk.com/Embed/Timeline/cc26215f-b821-4844-b44e-ec1eabc62104

Gilmer J. Vizconde

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If it was useful please mark as a solution and give me kudos  

[Anonymous]

What I'd like to produce is what the "solved" problem shows, but w/o the increase in arc angle of the notch so as to produce just an ever-expanding version of the initial notch. Ultimately it will accommodate a cone extruded from the large circle with a tab matching the notch (which works fine btw) in the outer extrusion to prevent the cone from rotating when fully inside the enclosure. I have tried using only arcs for both circular drawings to no avail. The extruded middle part shows what I want the outer extrude to accommodate.

[jeff_strater]

It is probably worth pointing out how Taper works with Extrude.  The original intention of providing a Taper angle in Extrude was to facilitate creating molded parts, which need some draft angle applied so that the part would come cleanly out of the mold.  Because of that, the taper angle is applied in opposite directions for "outside" vs "inside" faces of the extrude:

As @TheCADWhisperer says, it is not clear what your intention with this design is.  But, if you want to only taper the outer edges, and have the large hole with the small channel be untapered (just making a wild guess), you can do this with two separate Extrudes:

Jeff

[Anonymous]

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When I try to extrude the small arc part separately it fails. I'm
missing something.

[TheCADWhisperer]

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mack.mckinney wrote:  When I try to extrude the small arc part separately it fails. I'm
missing something.

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Can you attach this file here?

While I wait - the attached file is my best guess.

[Anonymous · Accepted solution]

The solution is:
1. Draw the rectangle, big circle and arc.
2. Extrude it all to the desired length.
3. Then extrude out the big circle and arc at the same time.
Done!
I was trying to do the initial extrusion to build the enclosure. By carving out the cylinder with the notch as above after a complete extusion seems somehow consistant with the ability to extrude the matching inside cone with tab.
Thanks to all who got me thinking straight. Man, this is an amazing forum!
Mack

[JDMather]

I would be really curious to see your solution - I must admit that I am still lost on the true design intent.

[davebYYPCU]

+ 1