Rigid Tapping G84 Canned Cycle

Rigid Tapping G84 Canned Cycle.

Let’s face it tapping on a CNC Machine can be a “right pain in the arse” as we say in the Midlands. But help is at hand. All you need is a bit of knowledge and the right equipment and it’s a dream, an absolute pleasure.

What is Rigid Tapping?

You mean you didn’t know? Well the first step is admitting you didn’t know.

Rigid tapping means the tap can remain rigid throughout the tapping cycle. It can be held in a chuck just like an endmill or a drill. The machine spindle locks in with the feedrate just like when you are screw cutting. You can buy tapping heads specially for this. They are no different to holding in a chuck but you get to use collets for holding the tap. These make it easy to change and it can’t spin.

Oh and you don’t need to remeasure the tap if you replace it.

So What Use Is This You Say

Well here are some of the advantages.

1. No need for expensive tension and compression tapping heads.
2. You can control the depth of the thread very accurately.
3. It is ok to re-tap the same hole if it needs to be deeper.
4. Peck Tapping of difficult materials is possible (Yes there is such a thing).
5. Quicker set-up times.
6. Feed is the same as the tap pitch.

But There’s a Catch

It’s an option. Sorry you might not have it.

Most modern machines do have Rigid Tapping as standard but the older the machine the less likely it is that you will have it.

Sorry but you need to look in those boring manuals.

Rigid Tapping G84 Canned Cycle, Fanuc, Haas, Mazak.

T06 M06 (M10 x 1.5 Tap)

G90 G0 G54 X50. Y50. S300 M03
G95 (Feed per rev)
G43 Z3. H06 M08
G84 G98 Z-15. R1. F1.5
X75.
X100.
G80

On some Fanuc controls you will need M29 for rigid tapping.

T06 M06 (M10 x 1.5 Tap)

G90 G0 G54 X50. Y50. S300 M03 (S300 M03 Optional)
G43 Z3. H06 M08
G95 (Feed per rev)
M29 S300
G84 G98 Z-15. R1. F1.5
X75.
X100.
G80
G94 (Feed per minute)

Just another interesting note (Read This G98 G99)

In the above cycle the tap will rapid down first to Z3. as in the G43 line. On beginning the cycle it will then rapid to what is know as the R Point. In this case R1. (one mm above the hole).

It will tap to a depth of 15 (Z-15). Depending on whether you programme G98 or G99 it will return to either the Z3. or the R1. before moving to the next position.

If you want to know more about G98 and G99 then read the article above.

Heidenhain Uses Cycle 207

Oh! And did You Know This??

G94 feed per minute (feed is in mm per minute).

G95 feed per rev (feed this amount every revolution)

These two G codes are your friend when you’re tapping or should I say G95 feed per rev is your friend.

Why?

When Rigid Tapping G84 Canned Cycle on a Fanuc, Haas, Mazak or similar control it is best to use G95. This means that when you programme your G84 (Tapping Cycle) your feedrate is your pitch.

The really great thing here is that if you change the speed of the tap you don’t change the feed because it’s the pitch.

Bet you have made that mistake before???
You change the speed and forgot to change the feed. We all know what happened next.

How easy is that?

Oh and don’t forget to change back to G94 at the end of the tapping.

You will notice the Heidenhain does this automatically for you.

On Machines Like The BMC 800 from Toshiba

This machine has the Tosnuc 888 control.

T06 M06 (M10 x 1.5 Tap)

G90 G0 G54 X50. Y50.
G43 Z3. H06 M08
G95 (Feed per rev)
M05
S300
M843 (Synchronous Rotation command)
G84 G98 Z-15. R1. F1.5
X75.
X100.
G80
M845 (Cancel Synchronous Rotation command)

When you don’t have rigid tapping you need a tapping head like this.

Notice how it pulls out when the tap stops and reverses.

Ok So what’s Going on Here?

1. Let’s tap a hole.
2. Start spindle forward.
3. Feed to depth at correct speed.
4. Stop spindle (tap starts pulling out).
5. Reverse spindle (tap pulls out a bit more).
6. Start spindle (Needs to reach speed).
7. Feed out of hole.

So the problem is that when the spindle stops, reverses and starts up everything goes wrong.

But this tension and compression tapping head can take up all the slack.

Not An Exact Science.

Definitely not, depths will vary. You will probably need to do some hand tapping too.

Tapping Clutches

These are special collets designed to slip at a certain torque. This allows you to get to depth without breaking the tap.

You adjust the collar at the front to give the required torque.

You can’t use these on Rigid Tapping G84 Canned Cycle because the last thing you want is for the tap to stop rotating.

Haas Have The Answer

Rigid Tapping G84 Canned Cycle, check out this great video on how to stop the machine half way through tapping.

Recover it without busting the tap!!

Ok So Let’s Talk About Peck Tapping

Fanuc (if you have the option) is G84.2 just programme your normal tapping cycle but replace G84 with G84.2 and add a Q value which is your pecking depth.

G84.2 G98 Z-15. Q5. R1. F1.5

Why would one want to peck tap?

1. Holes that clog with swarf.
2. Difficult materials.
3. To impress visitors.

Don’t Have It? Don’t Despair You Don’t Need It if You have Rigid Tapping

If you programme this.

G84 G98 Z-5. R1. F1.5
Z-10.
Z-15.
Z-20.
G80

There you have it Peck Tapping.

So you move to a position and it taps a hole 5mm deep. Because you are in a canned cycle it will repeat the procedure at Z-10. Z-15. and Z-20.

How cool is that?

Thanks For Reading

Don’t forget there’s loads more folks.

And a YouTube channel

Contact Me

Services offered at CNC Training Centre

Edgecam programming and training.

Classroom programmer training.

Onsite CNC Machine Training.

CNC Programming and Training on all controls and machines.

Mazak Training Fanuc Training

Don’t forget we offer training on all types of Mazak Machines and all Fanuc Controls

---