Bevel edge gear

[CB63]

I'm trying to figure out how to achieve the beveled edge on the attached file. I downloaded the original file from over a year ago and just recently started to play around with it in Fusion 360.

I extruded the projected sketch and then tried to apply a fillet to the edge but its not the same edge as the gear body. I also tried to chamfer the edge but ran in to issues. I've run out of ideas as to how to apply a 45 degree cut to the gear teeth.

This is just an exercise for me in Fusion 360 and not for any use in any application.

[g-andresen]

Hi,

Is that what you want to achieve?

günther

[CB63]

I'm looking for a beveled (chamfered?) edge of 45 degrees like this:

[davebYYPCU]

Revolve this type of profile, 

Might help....

[g-andresen]

Hi,

in steps:

günther

[g-andresen]

Hi,

here is a screencast and the file for completion.
Tip: Switch on design history

günther

[TheCADWhisperer]

Extrude - Intersect is easiest technique.

[CB63]

This looks close to getting what I need, however, I'm needing the length of the beveled face to not be quite so long as shown on the bottom of the gear. Does that make sense?

In other words I just want a short distance slope 45 degrees.

Thanks for the help so far.

[g-andresen]

Hi,

I´ve made a new construction with dimensioned bevel.

Screencast

Take a look at the dimensioned sketch and where I placed the construction plane.

günther

[CB63]

This looks good except that the dimension appears to shrink and grow around the perimeter as you rotate the gear view. It seems like that if you gave a driven dimension to go along with the 45 degree angle and then did a revolve the distance would be the same all the way around the perimeter. Are you seeing that as well?

[davebYYPCU]

Two things, 

Your gear is not on the document origin, so you have to draw and use your own centre line / axis.

Dimension my black line in the profile, and it will be uniform all the way around if you find the correct axis.

Might help....

[CB63]

The document origin issue should be fixed in the attached file. I was trying to follow along with your screen capture on how to create the sketch but I got lost.

I'd like to ask if you wouldn't mind sketching it out on the attached updated file.

Thanks.

[davebYYPCU · Accepted solution]

Here you go, 

Moved the body to the origin, with Move Point to Point.  (it was on centre but height was off.)

Turns out the tooth at the east position was on the origin plane as well.

Create Sketch on the XZ plane.

Project > Intersect the top face of the bevel and the bottom face of the gear, (purple lines - others were deleted)

Draw a vertical line from the top inside purple point to the bottom line, make construction, (Black dotted line to align the cut profile,)

Draw a 45 degree line from that intersection Length does not matter but not too short.

Draw a 3 point arc, both ends of the black solid line, and big enough to cover the cutting to do.

Use this profile for a Revolve Cut, 360 degrees.  Use Z Axis for the Revolve.

Right click on the body and set opacity back to 100% (changed for the picture...)

Edit sketch for your design purpose, bigger, smaller, new angle, etc.

Might help....

[CB63]

You knocked this one out of the park my friend! The narrative along with the file / sketch did it. The resulting revolve of the profile does indeed make a uniform angled cut consistently around the gear perimeter.

Thank you to all that took the time to offer up assistance.

Regards,

Chris

[TheCADWhisperer]

Extrude of circle is less work than Revolve of triangle.

Get lazy!