Internal Slot Toolpath with Lollipop Cutter

[morgantooldie]

Could someone guide me in the right direction to put a toolpath on this part? I cant figure out which toolpath is correct for this operation. The closest I have come is the "Trace" toolpath but it isn't correct. Thanks

[oscar-cadcampilot]

This type of feature needs a projection type toolpath. Not sure it's currently possible in Fusion 360.

[engineguy]

@morgantooldie 

Can be done using the Trace, but you will have to either create a slightly larger part using the "Scale" in order to move the toolpath outwards as there is no Radial movement option in trace, as has already been suggested there is not a dedicated toolpath for this as yet, anything used is a "workaround".

My preferred method would be to Sketch an Elipse, angle it to whatever you want and then duplicate it in the opposite angle as in the image below, then in manufacture you would select the Elipse for the Trace toolpath, just need a leadin/out enough to clear the inner wall, anyway, just an idea for you, it does work (workaround), just will need some trial and error to get the Major and Minor values for the Elipse correct in order to get the same depth of cut all the way round, as it appears to be an lubrication groove I don`t think a slight difference will make much difference, all depends on how much time you are prepared to put into it, does work, I have run a simulation using the two Elipse in the image 🙂 🙂

Not perfect but might just get the job done.

Hope that helps a little 🙂 🙂 🙂

Stay Safe

Regards

Rob

[Anonymous]

I was curious how it would work out, it's there theoretically but I have no clue about your material, speeds and feeds .... 

[Anonymous]

For the other curious minds, it looks like I deleted some of the clues in course of cleaning up so here is rest of the story.

With Trace you have to construct sketch to guide tool when there is no usable edge of model in sink with how you intend to drive tool.

I am using "tool on center" to drive tool and offset down in Z axis by ,1875 because tool is programmed from tip.

So I started by drawing a 3 point circle representing cutter at highest point on ellipse.

Next, I drew a line from middle points of intersecting grooves, created plane at 3 points, then ellipse using 3 points.

Offset ellipse inward by half the tool diameter and make entry and exit lines for cutter.

If cutting steel, you can duplicate tool path, leave small radial stock and do second pass.

[Anonymous]

There is a problem with mirrored tool path running in conventional mode, I saved sketch as DXF file, imported it into new sketch on same plane then rotated it to symmetrical orientation relative to original.

I dumped the pattern and generated new tool paths with clime cut direction for uniform finish all around, now I am done,... I think. 🙄

[seth.madore]

Well done @Anonymous and @engineguy !

I suspected Trace was going to be the only viable solution, but truthfully, I've not been able to play with the forums much this week; I've got some short cycle / tight tolerance lathe work that needs to get out the door by Friday.....

[Anonymous]

Not to worry Seth, we got your back (when possible),.... just be sure to promptly deposit my cut of profits  😁🤣😂😋

[morgantooldie]

I was able to figure it out. To draw it  (I started a forum in the design forum because that was hard too lol), I ended up making the bore initially smaller, drawing a line on an angle and using spplit face. Then used the pipe tool and cut the pipe from the bore. I extruded a bore through the part to finish the bore size and get the depth of the grease loops where I needed it. I had to make 2 bodies, exact copies, and leave the groove one way in body 1, and in body 2 I mirrored the first one and then deleted it.

Toolpath ended up being a trace toolpath and using z stock to leave (half of the cutter) and the radial (depth of the groove). Took me a while to figure it all out. Here's a link to the finished file. I've successfully made the parts! Thanks everyone for the input

[Anonymous]

I compared the two results for purely technical reason, if lubrication is indeed intended function, part will work either way but there will be instances where that will not be the case.

In my sample, tool precisely follows grooves which is evident in simulation, with model turned on, all groove edges are clearly in sink with machined edges.

I have no "stock to leave" in finish passes, clean and precise cut throughout.

In your sample, there seems to be some guess work involved in placing tool on right path, tool is violating lower end of the groove as marked in screenshot. 

In operation data, there are "stock to leave" values in finish passes that I can't associate with anything but fishing for matching tool path with groove geometry.

I don't dispute the fact that there are other methods of achieving same result but in this case I'll stick with my way because I am precision nut and if that feature had any significance in functionality of machined part I could defeat any quality control complaints by simply submitting prove of how it was programmed.

I will credit your way for using arcs in lead in and out although feed rate adjustment in my case would be adequate way to control tool engagement.