Rigid taping rpm

1. Diamond
Join Date
Sep 2002
Location
Lawrenceville GA USA
Posts
6,268
Post Thanks / Like
Likes (Given)
846
1370

## Rigid taping rpm

I would like to ask how do you come up with your feed for a tap when using a VMC. I currently use a chart supplied by one of the manufacturers to find a rpm and then I multiply that by the pitch of the tap. However, I usually wind up with some funky number and I try to keep my feedrate at no more than two decimal places.

I will wind up just playing with the rpm to get as close to an even number for the feedrate as I can, like 40ipm or 30.02 or something else that has less than two decimal places in it. Do any of you have any formula or better way to get these numbers other than trial and error? If I was a little smarter or actually remembered any of the math I took in school 25 years ago I might be able to figure it out myself...

My machine has a fanuc 21i by the way, do any of the other controls out there allow more decimal places for the feedrate and how accurate can the machine feed anyway?

Charles

2. Aluminum
Join Date
Aug 2007
Location
Sunnyvale, Ca
Posts
199
Post Thanks / Like
Likes (Given)
1
26
If it's a cut tap I'll go with either the mfg reccomendations or something I feel is reasonal. If it's a roll tap I'll usually run my rpm at 1000 to 1500. No matter what size or speed, my tap feedrate is always 4 places. HTH

3. Cast Iron
Join Date
May 2008
Location
Great State Of Wisconsin
Posts
444
Post Thanks / Like
Likes (Given)
0
7
Charles...you should be able to feed to more accurate than a 2 place decimal on the 21i control. Anyhow if you want to run your RPM based on the feed rate then it is just opposite of how you calculate your feed based on RPM.

Let’s say for example you want to use a 13pitch tap running at a even feed of 10ipm. Convert your 13pitch into decimal 1/13=.07692 now take your feed of 10/.07692=130rpm.

Feed = 1/pitch*rpm
Speed= feed/(1/pitch)

Stevo

4. Titanium
Join Date
Oct 2007
Country
SPAIN
Posts
3,661
Post Thanks / Like
Likes (Given)
2079
1368
Charles,
When cutting ally (luckily that's 99% of the time woohoo!), we run at 1000rpm and whatever the feed works out at (3 decimal places being metric).
That's for M2.5>M8 taps.
However, if the job is higher qty's, we will run at 1500>2000 rpm.

Just for a giggle, I ran the robodrill at 3000rpm and it was like a riveting machine.
It was sooo fast (minimal acc/dec-in/out) with perfect M3 threads.
Cheers

5. Diamond
Join Date
Sep 2002
Location
Lawrenceville GA USA
Posts
6,268
Post Thanks / Like
Likes (Given)
846
1370
On my 21i control the display only shows 2 decimal places so that is what I try to stick with. I am not sure if it will accept feedrates with more or not. Actually when cutting I know the CAM software I use will output larger values and I assume that they are just rounded off. I didnt know if that would affect rigid taping or not.

I guess most people just dont bother to worry about the decimal places, I just assumed that things would go better if I kept my numbers simple.

Charles

6. Diamond
Join Date
Nov 2004
Location
WI
Posts
4,718
Post Thanks / Like
Likes (Given)
472
1095
Originally Posted by barbter
Charles,
When cutting ally (luckily that's 99% of the time woohoo!), we run at 1000rpm and whatever the feed works out at (3 decimal places being metric).
That's for M2.5>M8 taps.
However, if the job is higher qty's, we will run at 1500>2000 rpm.

Just for a giggle, I ran the robodrill at 3000rpm and it was like a riveting machine.
It was sooo fast (minimal acc/dec-in/out) with perfect M3 threads.
Cheers
You know that that Robodrill will happily tap at 5,000 rpm don't you?
Stop being a wimp!
The 24,000 rpm unit is something to see at 8,000 rpm... 25mm deep, 20,000 holes to tap. Done!

7. I will wind up just playing with the rpm to get as close to an even number for the feedrate as I can, like 40ipm or 30.02 or something else that has less than two decimal places in it.

What fer machine doo you have with a 21i on it that does not have rigid?

I doo feed in IPM on an 18 w/o rigid with a tapping head and I just run the numbers and set the infeed just south of nominal so that I'm not pushing the tap. On the way back out I feed just slightly higher than nominal. It is the amount of dwell that you allow for the reversing part that is the wildcard. (rotating inertia of great importance here.)

But you SHOULD be feeding in rigid in IPR at a 4 place decimal.

----------------

Think Snow Eh!
Ox

8. Diamond
Join Date
Sep 2002
Location
Lawrenceville GA USA
Posts
6,268
Post Thanks / Like
Likes (Given)
846
1370
Ox,

The machine does support rigid tapping, as I mentioned in my reply earlier the control only displays feedrate with two decimal places. As a result I try to get my feed and speed set so that I end up with even numbers with two decimal places or less. Do I need to worry about that, it would appear from the responses I have seen so far that I dont need to be concerned.

As for supporting IPR, I understand that is a manufacturers preference whether or not your control will accept that. So far it appears that my machine will not support it.

Charles

9. Taken from an 18i lathe, but...

N4T808(1/2-28 TAP)
M203S300
X0Z12.9
M8
M29S300
G84G99Z13.59F.0357
G80
G98
M9

WHERE:

M203 = Sub spindle start CW
M29 = rigid tapping mode
G84 = RH Z axis tapping mode
G99 = IPR
G80 = Cancle cycle
G98 - IPM

What kinda MTB would go to all that werk and not have IPR as an option?

I honestly can't believe that "rigid" tapping would even werk in IPM. ???

Have you played with it and made darn sure that you have no G99? If not - maybe we all need to find a param for you to change?

-------------

Think Snow Eh!
Ox

10. Titanium
Join Date
Feb 2006
Location
Republic of Texas
Posts
2,475
Post Thanks / Like
Originally Posted by Ox

What kinda MTB would go to all that werk and not have IPR as an option?

I honestly can't believe that "rigid" tapping would even werk in IPM. ???

Have you played with it and made darn sure that you have no G99? If not - maybe we all need to find a param for you to change?

-------------

Think Snow Eh!
Ox
My Fanucs, OT and 18M, use G94=IPM, G95=IPR. I can't imagine a machine that will rigid tap not having IPR capability. The 2 place decimal display bothers me. That "should" be a regular parameter setting.

11. Titanium
Join Date
Oct 2007
Country
SPAIN
Posts
3,661
Post Thanks / Like
Likes (Given)
2079
1368
Originally Posted by 3t3d
You know that that Robodrill will happily tap at 5,000 rpm don't you?
Stop being a wimp!
The 24,000 rpm unit is something to see at 8,000 rpm... 25mm deep, 20,000 holes to tap. Done!
yeah yeah yeah, I know I'm a chickenshit!

12. I think you need a G95 (inches per rev) command somewhere just before you call your G84. Just remember if you're using inches per minute elsewhere in the program to set it back to G94 (as I often forget to do...).

From our 21i here:

N7(#10-32 TAP)
G55 G90 G95 T7 M6
G0 X0.500 Y-0.157 S350 M3
G43 Z0.1 H7 M8
G84 Z-0.625 F0.0313 (32 thd pitch = 0.0313)
Y-1.093
G80 M9
G91 G28 Y0 Z0 M5
...

I agree with alphonso. Our Daewoo sounds terrible if you try and rigid tap in G94.

-aj

13. Stainless
Join Date
Jun 2006
Location
Posts
1,824
Post Thanks / Like
Likes (Given)
573
308
For inch taps, I take the number of threads per inch and multiply that by 10 to get the rpm. Tapping feed is now 10.0ipm.
For a newer machine, multiply TPI by 100.
Therefore, a 10-32 tap would run at 32 x 100 or 3200rpm and feed would be 100.0ipm.
While this may not be optimum, you get the idea. Tapping feed is an integer and really easy to check at the machine.

14. Diamond
Join Date
Sep 2002
Location
Lawrenceville GA USA
Posts
6,268
Post Thanks / Like
Likes (Given)
846
1370
Jim,

Really simple idea, thanks for sharing that, if the speed is too fast just divide both equally and adjust the value.

How do you know if a machine will accurately rigid tap at 100ipm? Is there some value to look up in the manual that would offer that kind of information? I know many of the drill/tap machines can really book but I dont know how my machine would be able to do that or not.

Anyone have an idea on how to estimate what the real limit would be for taping?

Charles

15. Stainless
Join Date
Jun 2006
Location
Posts
1,824
Post Thanks / Like
Likes (Given)
573
308
It's hard to say just what the real limits would be for your machine. Let us know what model it is and someone may here may have the answer. We just received two new Haas machines and I got to see rigid tapping firsthand today.
Backing out of the hole at 4X the rpm going in was one of the first surprises that I had.

16. Titanium
Join Date
Oct 2007
Country
SPAIN
Posts
3,661
Post Thanks / Like
Likes (Given)
2079
1368
Charles,
Have a look at parameter 5241. The value is the maximum programmable rpm that the machine can tap at.
This of course is on the undrstanding that the machine has been servo tuned correctly...
But being an okuma, it should be ok.

PM me if you want a copy of some manuals.
Cheers,
Terry

17. Diamond
Join Date
Sep 2002
Location
Lawrenceville GA USA
Posts
6,268
Post Thanks / Like
Likes (Given)
846
1370
Thanks Terry, I will look at that and let you know what I find out.

Charles

18. Hot Rolled
Join Date
Feb 2007
Location
Georgia
Posts
728
Post Thanks / Like
Likes (Given)
0
35
Originally Posted by CBlair
Anyone have an idea on how to estimate what the real limit would be for taping?Charles
It's kinda like taking a curve on a motorcycle. The motorcycle is the machine, the tires represent the tap, the curve is the material. You only know the limit when you exceed it.

I use a method similar to Jim's and it has served me well on our Haas VMC's. I start with 30 IPM, multiply it by the pitch and see what the number looks like. Examples:

5/16-18 - 18 tpi X 30 ipm = 540 rpm
3/8-16 - 16 tpi X 30 ipm = 480 rpm
1/2-13 - 13 tpi X 30 ipm = 390 rpm
5/8-11 - 11 tpi X 30 ipm = 330 rpm

The above numbers are conservative in steel. You will note that they all work out to around 50 SFM. I do mostly one-off parts and can't afford to play with the numbers.

If the number looks wrong I increase or decrease IPM by some increment of 10 to get a sensible rpm. Example:

For 1/2-20 tap
20 tpi X 20 ipm = 400 rpm

Yeah, I know this doesn't strictly follow the rule that says you should always use the manufacturer's SFM recommendations. But it is a good job shop method for keeping numbers in your head for the most commonly used taps.

There is a similar method for metric taps. At 254 rpm the feed in ipm is ten times the metric pitch.

Thus, at 254 rpm:

Pitch (mm) Feed (ipm)
0.8 8.0
1.0 10.0
1.25 12.5
1.50 15.0
1.75 17.5
and so on..........

Now look at the rpm for the tap in question. You know an M6X1.0 will safely run at three times that speed. So multiply speed and feed by three and you have your numbers.

S254 F10. becomes S762 F30.

As with inch taps, your feedrates in steel will fall between F20. and F40. for nearly all tap sizes.
Last edited by doug6949; 08-29-2009 at 08:55 AM. Reason: BIG OOPS! 256 rpm should have been 254 rpm

19. Stainless
Join Date
Apr 2009
Country
State/Province
Ontario
Posts
1,555
Post Thanks / Like
Likes (Given)
534
486

20. Stainless
Join Date
Mar 2006
Location
Columbus, Ohio
Posts
1,115
Post Thanks / Like
Likes (Given)
3
124

## Rigid taping rpm

Wow, what a variety of figuring the speed for tapping.
First, the speed changes depending on the hardness of material, 1018 steel is tapped real conservatively at 30 SFM around 20 to 32 TPI, less if you do a rough thread, lets say 4 TPI.
Aluminum, of course, can be tapped at a higher surface foot value and in harder materials the SFM value goes down.
To get to RPM use this simplified method, it gets you real close.
Take the SFM value times 4 and divide that by the diam. of the tap. If it makes you more comfotrable, round it off to a nice number. The feedrate is either the pitch of the thread in G95 or the result of multiplying the RPM by the pitch in G94.
I have used a book coming from the "Machining Data Center" in Cincinnati for the last 30 years, it seems to be quite accurate. They are at www.cutdata.com .
The F value on Fanuc goes to 3 digits, so you can do it in inches per minute or inches per revolution, its either G94-G95 or G98-G99 depending on which G-Code system your control is set up for.
On my DVDs, all of this is on "Prep for CNC".
Heinz.
www.doccnc.com

#### Posting Permissions

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