G84 & G74 tapping cycle

[Karl_T]

I'm trying to write a Fanuc compatible tap cycle for my mill, so that a Fanuc mastercam post will work correctly. The format is:
G84 X_ Y_ Z_ R_ P_ F_ from what I've read.

First, are there any more optional parameters?


X,Y,Z, and R should be the same as all other canned cycles.

I have NO IDEA what P is.

I assume F is feedrate. If I'm tapping 1/2 X 20 threads, do I enter a .05 for inches per rev. or a 20 for threads per inch.

I assume G74 is just left hand, correct?


Thanks for the help.

Karl

[SnakeD0ct0r]

P is for a dewll, G74 is usully for a lathe, if you want to do a left hand thread program M04. Feed rate is in IPM, RPM*PICTH=IPM. So if you wanted to tap a 1/4 x 20 at 500 RPM the IPM would be 500*.05=25. X,Y,Z and R are programmed the same as in the drilling cycles, I usually start tapping .2 above my surface to make sure the spindle and Z axis have enough time to get synched, also if you are using a tension and compression tapping head, gives a little more room to make sure the tap is out of the hole before you rapid to the next location.

[Karl_T]

I'm setting up a rigid tap cycle where Z follows the spindle based on the thread pitch. What you're saying is for a non-rigid tap cycle. Is there an entirely different Gcode? Somehow, I need to pass thread pitch in the Gcode.

I'm trying to make this compatible with mastercam, I don't want to end up with a custom Gcode that needs editing every time its used.

[SnakeD0ct0r]

Usually there is a M code (M23 I think, it has been a while) that is out put with the spindle speed for rigid tapping. The feedrate should be the pitch .05, not the number of threads.

[stevo1]

It will depend on what kind of control you are using. Some controls are different. I have mostly Fanucs.

You need to use G84 for tape cycle. For my 16 series controls you need G84 along with M29 to create rigid tap. On the 15 controls I can use G84.2 and not use the M29. G73 should be your highspeed peck drilling cycle.

To figure out the feed that you want to go with your tap is all set by the spindle speed that you want to be at. If you are making a 1/4-20 thread you have to take 1" divided by 20 then multiply by the spindle speed. This should be your feed. Using a spindle speed of 25 your feed should be 1.25. If you need to increase or decrease your spindle speed or feed you have to recalculate one or the other.

Stevo

[Karl_T]

Originally Posted by stevo1 It will depend on what kind of control you are using. Some controls are different. I have mostly Fanucs. You need to use G84 for tape cycle. For my 16 series controls you need G84 along with M29 to create rigid tap. ... Stevo

I'd like to emulate the Fanuc 16 series from what you're saying. I'm sure mastercam can be set up to do that.

Do you have details about the M29 code?

Karl

[Mitsui Seiki]

You can use G84.2 with both Fanuc M15 and 16.
And if you want a peck cycle you write the code like this:
G84.2 X_ Y_ Z_ R_ Q_ F_ (Q for the peck depth)
It works on Fanuc M16,I'm not sure about 15 though.

[Karl_T]

Thanks about the tip on peck. I'll include that. My control doesn't do a decimal point after the Mcode. So, I'm looking for what might be in the M29 code.

FWIW, I got a trial of the Z axis slaved to the spindle done this morning before I had to go eat turkey.

Karl

[stevo1]

Originally Posted by Mitsui Seiki You can use G84.2 with both Fanuc M15 and 16.

Cool I did not know that. All my documents specify that the 16 series uses the M29. Nice to know.

Karl,
Do you mean your control does not take a decimal in the G-code? What kind of control are you using?
The M29 is just a rigid tap mode. I don't know the exact details of how it works. With the M29 and using the G84 this will sync your spindle and feed for rigid tap.

The G84 is a tap cycle. G84.2 is a rigid tap cycle. If only G84 is allowed then M29 is needed with the G84 to create rigid tap.

Stevo