Speeds And Feeds (hole saw)

[venomgrrrl]

I am running a CNC mill, and am going to use a holesaw (or annular cutter)
They are 2" (22 teeth) 2 1/2" (26 teeth) and 2 3/4" (28 teeth) and have a pilot drill
I am cutting thru 1/4" brackets, (cs aroudnd 80) and cannot remember the proper formula for feeds, though I do recall it has to do with the amount of teeth on cutter,
I am going to assume the RPM would be much slower than that of an endmill. Any suggestions?

[Mcgyver]

rpm = 4 * CS / Dia. CS= cutting speed and is a constant for each combination of tool and material being cut. this formula is basic to any machining operation, doesn't matter whether its drilling, turning, milling, whatever. volumes have been written on it herein.

I would suspect, that reality and theory are going clash in calculated a hole saw feed rate. if it did cut perfectly evenly, a theoretical chip load per tooth would generate a huge feed rate and corresponding forces on the cutter....however its not likely to cut evenly. other that experimentation, which is how I'd determine it on a manual machine, not sure how to otherwise advise for your cnc app - start slowly and adjust?

[venomgrrrl]

yea I did find the formula F= N x RPM x f (N=#of teeth f=feed rt. in inches per tooth)
but i have no idea what the f is for each tooth (trying to remember from school, is pretty small # like 0.01 or less, 1 thou maby?

[HapSmo19]

Assuming the hole saw is harder than the workpiece, I wouldn't start any faster than 40-50 SFM and .0005 per tooth. If it chatters, increase the feed. When it goes into catastrophic failure, use an end mill and interpolate it like they taught you in school.

[Geof]

Originally Posted by HapSmo19 ..... When it goes into catastrophic failure, use an end mill and interpolate it like they taught you in school.

This thought went through my mind. Have you done it, did it work?

Are you actually using a hole saw or one of those trepanning cutters, I forget the name at the moment. A trepanning cutter I would run at maybe 60% of the speed for a face mill of similar diameter and would reduce the feed per tooth to the same amount. That is if my machine could handle it.

[Mcgyver]

Originally Posted by HapSmo19 Assuming the hole saw is harder than the workpiece, I wouldn't start any faster than 40-50 SFM and .0005 per tooth. If it chatters, increase the feed. When it goes into catastrophic failure, use an end mill and interpolate it like they taught you in school.

you guys must be using different hole saws than I've ever found. I've used Starrett and there is no way they are cutting on all teeth, nor are the cutting in a very even circle....better suited for carpentry imo. AT 28 teeth, you're going to feed a 2.75" saw down at 14 thou per rev? can't see it, but hey I've been wrong lots before.

I've used a 4" hole to cut out a 90" section of 1" AL, crappy finish needing a skim with a boring bar and a white knuckle cut....i think Hap's right, if you've a cnc interpolate the cut.

[307startup]

Originally Posted by Geof This thought went through my mind. Have you done it, did it work? Are you actually using a hole saw or one of those trepanning cutters, I forget the name at the moment. A trepanning cutter I would run at maybe 60% of the speed for a face mill of similar diameter and would reduce the feed per tooth to the same amount. That is if my machine could handle it.

Geof, we used to use a hole saw on the live axis of our Daewoo Puma 400 at work for a job that we did about every 6 weeks. The company I worked for at the time manufactures aftermarket Jeep suspension components. We were cutting an offset radius that would have been about impossible to interpolate due to the amount of Y axis travel (without using the C-axis live & we didn't have Mastercam at the time). I had never seen it before, but it worked a charm. We used Starret hole-saws, 3" diameter. As I recall, the program we used it on used a 30 fpm feedrate, with a .002" chipload, turning at 1200 rpms. We could get 100 parts before we'd have to load a new saw. C-axis would turn 180* to cut the other side.

[Geof]

Originally Posted by WYLD .... We used Starret hole-saws, 3" diameter. As I recall, the program we used it on used a 30 fpm feedrate, with a .002" chipload, turning at 1200 rpms. We could get 100 parts before we'd have to load a new saw. C-axis would turn 180* to cut the other side.

High speed steel hole saws or carbide tipped? That is an astonishingly high sfm for HSS and to a conservative like me fast even for carbide.

[307startup]

HSS hole saw. Should have read 30 ipm not fpm...and the rpms were not 1200, but rather 600. I apologize, I had to look at my programming sheets to verify.

[HapSmo19]

Originally Posted by Mcgyver AT 28 teeth, you're going to feed a 2.75" saw down at 14 thou per rev? can't see it, but hey I've been wrong lots before.

I dont like to backpedal but I concede. 30 SFM and .0002 p/t would probably be a safer starting point. Although I cant think of a reason to even try to put holes in a piece of steel that way on a VMC. I can't imagine any advantage but.....if I could.....maybe lathe part-off tools can be replaced with Sawzall blades and just rapided back and forth.......

The possibilities are endless.

[GaryCorlew]

This is most likely what she is asking about annular cutter/slugger cutter, I have used them in vmc but it has never gone very well. When I did use them I used low rpm and very slow feed. I do not and will not use them anymore, I now use spade drills