Helix bore improvement.

[kunfuzed]

I would really like to see an option in Helix Bore to bore down, then do a circle mill at a desired finish pass at the bottom.(Or if it already does this I'd love to know how)

 

Is there an ongoing improvements thread I could post this in, or is it worth emailing to qc?

 

Thanks.

[Tony35]

quote:

---

Is there an ongoing improvements thread I could post this in

---

LINKY

[Jaz]

You can do this using contour/ramp instead of helix bore. Choose multi passes and check "final depth" in the "machine finish passes at" box.

[gargodude]

I use helix bore all the time. The confusing part is that they designed this cycle around a line of tools that many of us have never heard of, which require that the finish pass comes out of the hole, rather than into it. I use this with "peckerhead" endmills, which are simply a regular 3 or 4 flute carbide endmill relieved by about .010-.020" so that only about 30-50% of the diameter of flutes remain at the end. I also like to put a small radius on each corner for a longer lasting tool. The relief keeps the tool from rubbing, which prevents tapered holes.

 

To make Helix bore work right, just uncheck the box for "finish passes" and do 2 "roughing" passes about .0002-.0005" apart. The tool will then only spiral INTO the hole. Check "Perpendicular entry" so your radius comp will work correctly and use a 45 degree entry/exit arc sweep for a smooth blend in and out. If you use the "peckerhead" tools, you won't have to make a complete pass around at the bottom of the hole. I usually set the "rough pitch" to about 20-50% of the tool's "head" length, depending on the material and the rough stock amount. For small holes, I check the "start at center" box. I had a whole bunch of these endmills made for different size holes and they work great. I can bore holes down to about .120" dia. at up to 5X depth and control hole size to less than .0001", consistently, from hole to hole, without playing "reamer roulette" on expensive parts.

[bob flat]

We are interested in helix boring for bushing holes and dowel holes from 3mm to 50mm or so. Is there a place to buy "peckerhead" mills? I am afraid to look for them on internet because i may get my pp slapped for it. Is there another name for them or a company? I reread the post above and see you are making them, relieving them yourself.

[GoetzInd]

quote:

---

without playing "reamer roulette" on expensive parts.

---

At least it keeps the day exciting.

 

We do the same with endmills here. We just grind down the flutes on a Dekel tool grinder.

 

Mike

[gcode]

quote:

---

The confusing part is that they designed this cycle around a line of tools that many of us have never heard of, which require that the finish pass comes out of the hole

---

I wrote this up as a bug during the X3 beta cycle.

Got a bug number and everything..

Maybe they need to add a switch to control

the finish pass is top to bottom

or

bottom to top

 

I have never heard of "peckerhead" endmills and as previously mentioned, googling

"peckerhead" would probably return some

undesireable results

[gargodude]

"Peckerhead" is not an official name. It was what my cutter guy called them when he made me some last time. Anybody with a surface grinder, a Spin-Dex and a narrow diamond wheel can make them for you out of existing end mills. Call a tool and cutter grinder.

[gcode]

as follow up on my bug report..

it has been changed to an enhancement request..

so that helix bore will have a switch..

to control the direction of the finsih pass..

from bottom -- up for peckerhead cutters..

and top down for regular cutters..

[bob flat]

Got x3 today and looked in help menu for helix bore. Mastercam says to use felix mills from Dapra corp. I looked at them and they start at .5 inch dia. Looks like smaller holes will be done with relieved end mills.