Post By Curt B
Tapping speed and feed formula needed
I'm looking for a formula to plug in proper feeds and speeds on a cnc lathe that does not have rigid tapping.
I'm trying to cut a 1/4-32 ID thread with a tap and have no clue where to start for rpm and feed rate. (floating tap holder)
So if anyone could punch up this example and show me how to you got the feeds and speeds so I can learn to use it properly that would be most appreciated.
I get my tapping SFM by looking at Vega Tap's recommended SFM sheet.
Surface footage info is available from most tap mfgr's.
As far as FPR goes I use the pitch of the tap. But if you are using a floating (tension/compression) holder, then you might want to feed in a bit laggin of the pitch.
IE 1/4x32 tap = 1/32=.03125" per revolution So for a T/C holder I might feed in at .03 IPR, and feed out at .03125"
So for 1000RPM, to feed in @ 30 IPM, and feed out at 32.IPM.
(1000rpm x .03" =30 inches per minute)
1/4-32. Is that for a glow plug?
Not that I know of.. just a feature on a part for a customer.
Originally Posted by 3t3d
Program a slower feed rate on the way in and the correct feed rate on the way out.
You can easily figure out how far the tap holder will extend by figuring the number of turns you want to cut. Let's say you want the tap to extend 1/4" on the in feed, and you want the tap to go 3/4" in.
1/32 = .03125
.750 / .03125 = 24 turns
.250 / 24 = .0104... so reduce the feed rate on the infeed by .0104.
G97 G00 X0 Z.25 M03 S200
G01 Z-.750 F.0209
G97 G01 Z.375 F.0313 S200 M04
Clack, tap holder snaps back.
Originally Posted by Nick H
In this case the time your spindle takes to slow down, reverse direction, and get back to speed are what will determine what you can use regardless of what's right for a given tool/workpiece material. The faster you go the worse it is.
Last edited by Curt B; 11-04-2008 at 11:48 AM.
I bet it is.
Originally Posted by 3t3d
Originally Posted by Curt B
Yeah, that's why I said 200 rpm. I also believe M05 between the two feeds is the best way. I've tried going straight from M03 to M04 and even at low rpm it sounds a little clunky. You'll have to try it and see, Nick.
The best way I've found is to feed in at 90-95% of the thread lead going in. The way out I feed at 100% but it doesn'y matter much either way.
Also you should use G32 instead of G01. This way if some bonehead has the feed rate overide turned up or down it won't break anything. Most controls execute the M05 after the commanded position has been reached. So the best way to program is like this:
Assuming 85 SFM for mild steel - 85/0.25*3.82=1299
Feed rate - 1/32=0.03125 0.0325*.95=0.0297
Hole depth = .5 so take .5*.95=0.475 and use 0.475" for your programmed Z-depth
G0 X0 Z0.08;
G32 Z-0.475 F0.0297 M05;
M04 Z 0.08 F.03125; (G32 is modal here)
You can also put a dwell in between the two G32 lines. Most small lathes don't need it, but a larger lathe with a big chuck might need a little time to stop before the spindle reverses. In that case program your approach further away and you depth shallower and use the Z-axis offset to bring the depth in.
SwissPro, you nailed it.
I thought I remembered M05 being on the end of the feed line but I wasn't sure. That does work excellent. Also I forgot about changing the depth of feed!
So, if for example, I wanted to tap with a 1/2"-14, i'd divide 1 by 14 (because there's 14 threads per inch?), then that would be ~.071 IPR.
Originally Posted by doug925
then i multiply the RPM i want, based on the recommended SFM for said material/tool (where the hell would I find that?) times the IPR, and I have my desired feedout-feedrate? Ig i'd round down for my feed-in feedrate, so .07 IPR?
Originally Posted by apestate
if using a spring tensioned tap holder then yes you can use different feed rate going in then coming back out
if using a rigid tap holder i would go exactly correct feed rate myself . kind of important to mention tap holder type