Rigid tapping

[Frank]

Hey all: I am programming a new machine, that has rigid tapping. I am used to using G84, and figuring out the feedrate and spindle, or in some cases, tell Mastercam the TPI and let it figure it out. I know a little about using a G841 but the manual has something about using a G95 and an E, or something like that in the same block. If somebody could show me what their rigid tapping code looks like after it's been posted, I'm sure I could figure the rest out. Also what kind of feedrates would you use on aluminium, say with a 3/8 - 16 tap.

 

Thanks,

Frank

[Guest CNC Apps Guy 1]

Here's a snip from my machine

 

N22G95 (IPR FEED)

N24M29S400 (SYNC SPINDLE AND AXIS)

N26G98G84Z-1.R.1Q.3F.0625 (CANNED CYCLE)

N28G80M9 (CANCEL CANNED CYCLE AND TURM OFF COOLANT)

N30G94 (IPM FEED)

 

HTH

[cadman03]

3/8-16

 

speed to start : 160

feed : 10 ipm

 

s160 M3

G98G84.1Z-.3R.1F10. ( Matsuura machine with 15M)

G80

[crazy^millman]

Well I would tap at 1500 rpms if it were me. I would also use a tin coated tap with plenty of coolant is going deep I would peck tap it also.

 

I have about the same code as Jaems excpet mine is for a Fadal.

[Frank]

Thanks all...James is this suppose to be a G841, and is it because of the G95 in the beginning block that your control reads the "F" as pitch? And is the Q.3 for peck tapping ? Also I'm checking to see if I need to use the M29.

 

 

" N26G98G84Z-1.R.1Q.3F.0625 (CANNED CYCLE)"

 

Thanks again

[Racer X]

G95 on my Okumas means inches per revolution feedrate. In that case, yes the F value would be the pitch (.0625 for 16 tpi). The nice thing here is not having to calculate the feedrate again when increasing spindle speed. Make sure you use G94 after the tapping cycle to go back to inches per minute feedrate on your next operation. I haven't been around any other machines for a while. So, this could be a pointless reply on my part. I also would use about 1500 RPM.

 

[ 01-27-2004, 01:01 PM: Message edited by: Moto GP ]

[Frank]

Millman are you for real on that 1500 rpm's ? That's what I am looking for ! Normally I program taps at about a 25. IPM feedrate using a tapping head. 1500 RPM's would be 93.75 IPM..I like it ! The holes are not to deep...1" so I don't need to use the peck cycle, or how deep should I be before using Peck.

 

Thanks all

[Guest CNC Apps Guy 1]

quote:

---

James is this suppose to be a G841

---

No, not for my machine (Mori Seiki SH-8000 with Fanuc 16iMA Control)

 

quote:

---

and is it because of the G95 in the beginning block that your control reads the "F" as pitch?

---

Affirmative.

 

quote:

---

And is the Q.3 for peck tapping ?

---

Also affirmative. I always use peck. Costs me a bit of time, but in the 6 months this machine has been running with the same 1/4-28 STI tap. Probably 20-30 holes per day. Just broke it the other day. I'm all about stability in my cells. I mean don't get me wrong, I push it hard but the process is stable.

 

quote:

---

Also I'm checking to see if I need to use the M29.

---

This will be machine specific. Some builders write their own canned cycles that use another variable to define Rigid Tapping or otherwise.

 

HTH

 

[ 01-27-2004, 01:36 PM: Message edited by: James Meyette ]

[crazy^millman]

Yeah I am very seriuos. 1" deep in alum I would be using a OSG modifed bottom Hy-Pro sprial tap. I think you will find that it kicks seriuos but.

If you tap to slow with soem taps you will get a ripping action verse a cutting action. You then of course have the other side of the coin to fast and that will suck but if the machien can handle it then go for it. Most book recommend 83 ipm on threads 16-24. so you are about 6% over the book at the feed rate. I use the book as a low start for just about any thing. I use to cut CRS with a face mill at 900 sfm. for roughing and 1350 SFM finishing. I would burn up some inserts of cousre but I would gain days on jobs that other were doing at the recommend speed and feeds and only be about 100 dollars in burnt-up inserts. If you take a normal shop rate I made $2000 to $3000 more than other guys with the same tooling only spending $100 to $300 dollars more in inserts and things like that.

 

 

Time is money and money is time. If you save one hour on a Job you don't gain one hour you gain two hours the one you saved and the one hour you got put on another job. I ask you how much time would you save if ytou just increased all of your speeds and feeds by 10% in one week and then how much more did that cose you in tooling I think if most looked at it with the Real Money idea verse the penny wise dollar dumb that alot do they would see the error in their ways. I understand that tooling cost money but if you are getting it done faster and the time saved greatly offsets the tooling cost then not to is crazy in my book.

 

[ 01-27-2004, 04:49 PM: Message edited by: Millman^Crazy ]

[Guest CNC Apps Guy 1]

For attended operations I agree with Millman. For unattended operations, it's best to be a bit on the conservative side because you want a stable process that won't give you a ring at 3:00am.

[crazy^millman]

+1000 on James there. If I am writing program that are unattend I do take it easy cuase if a tool break then yeah that sucks.

 

 

Good Point James!!!!!!!!!!