G Code Tapping Problem

[Wally]

The main man is out today and I`m lost. Could someone please help? We are running a Matsuura MC-500V. The operator has a Tapmatic head for an 8-32 helicoil tap. He`s asking me for what kind of "G" code to use. Thanks up-front for any help.

[mayday]

auto reverse head?

use a G01 with feed to match the thread pitch

 

feed to depth and feed out

[Philcott]

When we use our reversing head we start the tap cycle about .45" above the part to allow for the tap to get out of the hole before the machine moves to the next hole. There is a time lag when reversing.

 

Phil

[Wally]

I just ran across a list we have here. It`s showing a G84 for tapping. Now I`m really confused. Yes, it is auto reverse. Thanks MayDay

[Philcott]

Wally,

 

Just to add more confusion. We use G74 which is a "tapping head" cycle for out Fadal.

 

Phil

[Toolfab]

Here is the code I use for tapping

 

N2350 ( DRILL/MISC OPER W / T7 .1181 DIA )

N2360 T7 M6

N2370 S240 M13

N2380 B0

N2390 G84 Y0.2 Z-0.2 F5 I2.4

N2400 G79 X-0.149 Y0.0005 Z-0.125

N2410 G0 Z2

 

I don't know if that will help, but it may be a start.

[robk]

quote:

---

It`s showing a G84 for tapping.

---

G84 is a right hand tapping cycle

G74 is a left hand tapping cycle

 

Never used an auto reverse head, so have no clue as to what applies there.

[Noel]

We run a g85 with the feed reduced by 5 % and as Phil said start .4 or .5 above the part. Also if it is a blind hole stay shallow on the first one and check the depth.Also because it is not a g84 you must make sure the spindle and feed rate overides are set to 100% because the spindle isnt synched in a g85 cycle.I learned that one the hard way.

 

 

HTH Noel

[?Mark]

Some of our older machines do not have rigid tapping so we use G85 (feed in feed out)

Also with heads like this adjust R a little higher then normal (R.25)

Next thing I do is run rpm a little higher than calculated.

 

For example fo 2-56 S650 F10.8

 

G85G99X.1Y.3052Z-.14R.25F10.8

 

Hope it helps, Mark