[Snowie]

Hi All
This is probably a no brainer to you clever people.
I have a number of grease galleries to drill some shafts 5.5mm Drill X 90mm deep
I need a example of some code do a drill retraction to clear the swarf

I can peak drill with a G74 down to Z-30.00 fine but how do i go deeper and clear the swarf with a retraction to Z0.50 and rapid back to hole bottom

With a G90 it rapids out fine but goes back into the hole at the programmed feed rate (takes ages)

I'm running a Fanuc 6T Lathe

Thanks
Snow

[txcncman]

I take it your lathe does not have G83 drilling cycle. Does it have custom macro capability? Do you have enough Z travel to clear the drill by its own length from the front of the part?

There are many threads on CNCZone about deep drilling. Just look for them using the custom search box at the top right of the page.

[Snowie]

I take it your lathe does not have G83 drilling cycle. Does it have custom macro capability? Do you have enough Z travel to clear the drill by its own length from the front of the part?

There are many threads on CNCZone about deep drilling. Just look for them using the custom search box at the top right of the page.

Sorry no G83. My machine is a oldie...Still a goodie thu

Yes i can call a custom macro P(prg number) (M99 to return to the prgm that called it)

Yes there is enough length in front of the workpiece

[txcncman]

You can tackle this problem with a custom drill macro. Search some of the threads about drilling macro here on CNCZone.

You can also do a sub program with looping to get full retraction. It is a little tricky but doable. In the main program you would put your sub call with repeat X times:

G00 X0. Z0.1
M98 P1000 L51
G00 G90 Z0.1

Then the sub would look something like:

G01 G91 Z-0.1 F0.004
G00 Z5.
G00 Z-4.9
G01 Z-0.1 F0.020
M99

The above should drill a hole 5.0 deep. It loops 51 times to account for the Z0.1 start point.

[Snowie]

Thank you!!!!!!!!!!!!!!!!!
This is a massive help

[sinha_nsit]

A clever program indeed.

[txcncman]

Thanks. But I did not invent it. Was taught by some old guy years ago.

[Snowie]

It's got that 'Kiss' thing written all over it

[MetalZilla]

Hi,
try this Drill Pecking Calculator: Drill Peck Calculator

[g-codeguy]

Yes i can call a custom macro P(prg number) (M99 to return to the prgm that called it)

Not really sure I fully understand this statement. Yes you can call a macro program with a P, but the format for using a subprogram is exactly how you describe. It doesn't mean you have macro capability. Do you truly have Macro B? If you do, then I have a macro program to do what you want. Also should you have Macro B, will it accept an IF/THEN statement? My macro program would require modifying if not.

[Helman Jr.]

You can also do a sub program with looping to get full retraction. It is a little tricky but doable. In the main program you would put your sub call with repeat X times:

G00 X0. Z0.1
M98 P1000 L51
G00 G90 Z0.1

Then the sub would look something like:

G01 G91 Z-0.1 F0.004
G00 Z5.
G00 Z-4.9
G01 Z-0.1 F0.020
M99

The above should drill a hole 5.0 deep. It loops 51 times to account for the Z0.1 start point.

Of course intelligent use of G91 always works, there are multiple such examples when Incremental programming helps solve very complex calculations.

Helman
cnc programming tutorials