Tapping speed and feed formula needed

# Thread: Tapping speed and feed formula needed

1. Aluminum
Join Date
Jun 2007
Location
Westfield, WI
Posts
85
Post Thanks / Like
Likes (Given)
0
0

## 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.

2. 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)

Doug.

3. Diamond
Join Date
Nov 2004
Location
WI
Posts
4,571
Post Thanks / Like
Likes (Given)
366
1010
1/4-32. Is that for a glow plug?

4. Aluminum
Join Date
Jun 2007
Location
Westfield, WI
Posts
85
Post Thanks / Like
Likes (Given)
0
0
Originally Posted by 3t3d
1/4-32. Is that for a glow plug?
Not that I know of.. just a feature on a part for a customer.

5. Stainless
Join Date
Mar 2003
Country
UNITED STATES
State/Province
Utah
Posts
1,057
Post Thanks / Like
Likes (Given)
51
15
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
M05
G97 G01 Z.375 F.0313 S200 M04

Clack, tap holder snaps back.

6. Originally Posted by Nick H
I'm looking for a formula to plug in proper feeds and speeds on a cnc lathe that does not have rigid tapping.

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. Reason: spelling

7. Stainless
Join Date
Jun 2006
Location
Posts
1,731
Post Thanks / Like
Likes (Given)
478
265
Originally Posted by 3t3d
1/4-32. Is that for a glow plug?
I bet it is.

8. Stainless
Join Date
Mar 2003
Country
UNITED STATES
State/Province
Utah
Posts
1,057
Post Thanks / Like
Likes (Given)
51
15
Originally Posted by Curt B
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.

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.

9. 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

G97M03 S1300
T1212;
G0 X0 Z0.08;
G32 Z-0.475 F0.0297 M05;
M04 Z 0.08 F.03125; (G32 is modal here)
G04 P1000;

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.

10. Stainless
Join Date
Mar 2003
Country
UNITED STATES
State/Province
Utah
Posts
1,057
Post Thanks / Like
Likes (Given)
51
15
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!

11. Originally Posted by doug925
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)

Doug.
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.

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?

12. Diamond
Join Date
Dec 2008
Country
UNITED STATES
State/Province
New York
Posts
8,158
Post Thanks / Like
Likes (Given)
0
2168
Originally Posted by apestate
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
M05
G97 G01 Z.375 F.0313 S200 M04

Clack, tap holder snaps back.
.
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

#### Posting Permissions

• You may not post new threads
• You may not post replies
• You may not post attachments
• You may not edit your posts
•