What's new
What's new

Rigid taping rpm

CBlair

Diamond
Joined
Sep 23, 2002
Location
Lawrenceville GA USA
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
 
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
 
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
 
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
 
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!
 
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? :eek:

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
 
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
 
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? :nutter:



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

Think Snow Eh!
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? :nutter:



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

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.
 
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
 
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.
 
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
 
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.
 
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:
For rigid tapping you need to set a code. You cannot rigid tap with a standard floating tap formula. Example a 13 pitch thread. 1/13xrpm will bust your tap depending on depth. The simple fact that you program 2 decimal places for your feed. I don't believe your control only reads 2 decimal places otherwise it wouldn't have tapping period. It may display it as 2 but have you programmed 4 decimal places and watched the display? Maybe its only displaying 2 cause you only programmed 2. Either way even if it only does display 2, most likely its reading more. If you tap a 1/2-13 with a floating head, then this feedrate will be no problem. .077. If you try to rigid tap with this feedrate, you might as well say bye to your tap. Best thing I would reccomend is to look at your manual where it shows rigid tapping (as you said it supports) and look for the code that activates the rigid tap. Then it should calculate the feed automatically based on your pitch. As for RPM as someone already mentioned, look up the mfg sfm chart.
 
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
 
Wow, what a variety of figuring the speed for tapping.

This is because he was asking about how many decimals his machine can handle. The rest of your post (my opinion anyway) is making everyone else at PM sound as if they are all new apprentices. I'm sure the OP already knows about the basic rpm formula. Besides he wasn't even asking about speeds to begin with. I'm sure he also knows that the speed varies on different material, again not what hes asking. Not to sound like an ass, but your response was pretty much "useless" as it didn't touch any of the questions he asked except for that his machine will accept more than 2 decimal places.
 
My thanks to all of you who posted responses, the variety of ideas is just what I was hoping to see. There is no black art to what we do and there is no one only best way to do anything. We all learn by working with others and from our shared experiances. I value the opinion of everyone who posted and thank you all again.

Charles
 
Hi, I've been following this thread now, and dont have any experience with programming a tapping cycle, but today I was working on a job in stainless steel where we are tapping each end, one end 3/8-16 and the other 1/4-20. The 3/8-16 worked fine, but the 1/4-20 taps kept breaking left and right. The 3/8-16 was programmed for 75 RPM, and the 1/4-20, 50 RPM (G97). Reading this thread these sound really low. Could these RPMs contribute to breaking taps? For reference, I am tapping on old Hitachi Seikis, TS15.

Edit: Actually on the trouble tap, it is in a floating holder, the other is in a rigid holder.
 








 
Back
Top