Lollipop Deburr Crosshole

[alwall]

Happy Saturday! Got a tricky deburr question for those who like a challenge. I machine quite a few parts that have intersecting holes. On center is usually no problem and most circular/elliptical intersections I figure out...however, this one has me stumped. Got some flat bottom holes and some double intersecting holes (football shaped) that need a light edge break.

3D contour is not doing it for me and neither is Trace. 3D contour looks good, but gouges the part (randomly) and takes a while. What I really want is a Trace style path that will lead in/out in X/Y, run the traced outline of the hole and retract. Tool Comp on center is the only way the path looks okay but with no leads. If I put comp on, it's all weird. See below for some pics and I attached a condensed file a what I'm dealing with. Any help appreciated. 

Trace (No comp/No Leads):

Trace (Comp On...inside the part!)

[a.laasW8M6T · Accepted solution]

So I model a shallow chamfer on the part and use the Flow toolpath

Short Video on how i do it:

[alwall]

@a.laasW8M6T 

Thank You! I really appreciate you taking the time to post a detailed video with my part.

I had to play with the tolerance some and use a smaller lollipop on the D shaped holes, but this solved my woes of having to flex hone or otherwise hand deburr these parts. 

[alwall]

@a.laasW8M6T 

I'm at it again with a new cross hole deburr issue. This one has two different inner diameters that the port intersect. I tried the previous method with shallow angle chamfers and I cannot get the vertical surfaces to play nice. My next go-to for stuff like this is a double angle chamfer cutter. They usually work great...on 2D backside deburring...but flow will not accept "form mill" as usable tool. Any ideas on how to force lollipop to work or another path that will can handle to double angle cutter (preferred)? Can I lie to the software somehow to get double angle to follow that path?

[a.laasW8M6T · Accepted solution]

Yea, you cannot use form tools with 3d toolpaths really, they work ok with most 2d toolpaths.

I do some undercut chamfers on sprockets with a double angle cutter and trace, but its not perfect and they are relatively shallow angles. once you get to steeper angles and radii like in this part trace will just gouge massively.

Flow does work here if you deselect the vertical faces, you can't really machine them with any tool anyway(from that orientation) because of the sharp corners, so you may have to accept that those edges will need some hand work

[alwall]

@a.laasW8M6T
As always, thanks for your input!
There is a small chance I can sneak in through the cross hole with another tool and get this done. These are machined in a horizontal. Customer will allow a sharp corner (possibly small burr), just no heavy/hanging burrs. Got hundreds to do, so I better get crackin'.

[paffmfg]

I would like to bump this to the top of the board. I have tried to get this to work with my parts and I can't seam to get it to work. The interface for Flow seams to have changed enough that the above video is not useful. At least not of me.

[a.laasW8M6T]

Yea that was with the OLD Flow toolpath which is technically still available but I wouldn't recommend it.

I would use Geodesic(set to blend) now, but I don't think you will be able to machine the 45° chamfers you have modelled, note how in My video I model them at a shallower angle.

With geodesic you can limit the number of stepovers to 1 if you only want to do one pass

If you are still having trouble you can upload your file here for us to look at.

[paffmfg]

I tried that geodesic path and it looks like i at least get a path that pretty much makes sense now. I tried setting the path type to blend under the geometry tab but it gave an error. No problem though this will get me another 80% closer.