[SCzEngrgGroup]

There's a diagram of the innards in the manual (PDF): http://www.rockford-ettco.com/Downlo...5000-16000.pdf

That appears to have conical friction clutches, rather than the dog clutches in the Chinese ones. A much better design, I think. I find the most common time for the tap to break with the Chinese ones is when the reverse clutch first engages, as there is a torque spike, due to the very sudden engagement. The friction clutch would allow a more graceful engagement.

Regards,
Ray L.

[RussMachine]

Superman,
So it's ok to use traditional G84 canned cycle?
I read in the manual, and on Tormach's website not to use it. ??????
G84 would be a lot easier than the long-hand version.
I'll give it a try on a piece of scrap.

[Superman]

Superman,
So it's ok to use traditional G84 canned cycle?
I read in the manual, and on Tormach's website not to use it. ??????
G84 would be a lot easier than the long-hand version.
I'll give it a try on a piece of scrap.

Going by the

Tormach suggests using long-hand code instead of G84, because the Tormachs don't have TRUE rigid tapping..

you are NOT "fixed" or rigid tapping if you use a T/C holder....IMO.... you can use G84....yes, try it out by all means. You have to be confident in your tooling.

I worked a Fanuc control yhinking it had the rigid tapping option. was tearing the threads apart ( tap held in collet chuck )
ended up getting a T/C holder, now no problems. Even using an M16 tap

[olof]

There is no reference to G84 in the Tormach manuals. There is G83 and 85.

Does Tormach support G84 and how do you program it?

[RussMachine]

Olof,
You're right, here is no reference to G84 in the manual.
However, there is G84 on the MACH3 on-screen list of G-codes, but it has a side-note "Not yet implemented."
I'm gonna do a test-run of a G84 cycle, with my T/C head, and see what happens.
I'll post my results.

[RussMachine]

Alright, I tried my test-run of G84.
I ran it without cutting any material, just cutting air.
It was odd.
There was a really long pause (about 6 seconds) between finishing the hole, and locating to the next hole.
????
It fed down, instant reversed, then fed out.
HOWEVER, it looked like it started feeding out, BEFORE the spindle reversed (Maybe half a second delay).
It looks like it might work with a T/C Head, I'm a little scared to try.
Here's the program I ran:
(Test G84 tap 1/4-20)
M6 T1
M3 S600
G90 G54 G00 G43 X0. Y0. Z.5 H1
G84 G95 X0. Y0. Z-.5 R.1 F.050
X1.
X2.
X3.
G80
M5
M998
M30

[vertcnc]

I though there was a M29 along with the G84 for rigid tapping with a fanuc (mach3) control. Which I believe has the reverse spindle function within. Not sure though.

[SCzEngrgGroup]

Try adding a P0.5 or P1.0 to the G84 line. That should make it pause at the bottom of the hole to let the spindle reverse before starting the retract.

Regards,
Ray L.

[RussMachine]

I though there was a M29 along with the G84 for rigid tapping

Ahhh.. Maybe I should try the suggestions.
M29 (Rigid Tapping) and put a P1.0 in there also.
More experimenting tomorrow

[Superman]

The Fanuc does use the M29 with the G84
- the M29 is executed before the cycle, but I have found out the hard way ....it is not a true rigid tapping setting code for a machine that does not have the rigid option
but, it does make the tapping cycle flow better.

The way I would program a tapping cycle

()
M6 T1  ( 1/4 UNF TAP )
()
G90 G54 G00 X0. Y0.        ( goto XY origin )
M3 S600                    ( set speed, turn ON )
G43 Z.5 H1 M8              ( take up tool length, coolant ON (if required))
M0                           ( program stop, to clear any chips from the holes, apply cutting oil, etc. ) 
G95 M29                    ( feed per rev, tapping mode )
G84 X0. Y0. Z-.5 R.1 F.050 ( tap cycle)
X1.
X2.
X3.
G80 M9            ( cycle cancel, coolant OFF )
G94               ( FEED / MIN )
M5
M998
M30

The red code I place on all programs before the toolchange, for safety. The main one is putting the feed BACK to "FEED per min"

Some controls can use a Q value on the G84 line...for a peck cycle... use with caution as it may not work
P is a dwell at the Z depth of tap cycle, not each peck ( P not usually required )
ie G84 Z-1.5 P0.2 Q0.75 R0.2 F0.050 ( peck every 0.75" from R plane until Z depth )

The other problem you may encounter is that the tap is not synchronised, so I would advise not to run the tap down a hole that is already tapped in a previous cycle.

[mountaindew]

Is there a way you can get Sprutcam to post your subroutine for tapping operations? To be honest I'm still working on that part, though I can't give you specific guidance as I run BobCAD and LinuxCNC, and haven't bothered since I don't do a lot of tapped holes. Well, I didn't until I made a fixture this weekend with 60 10-32 holes, which made me think it's time to figure out how to get Bob to post my subroutine instead of rigid tapping G-codes. As it is, I do it kind of like you say--let the CAM drill everything and then do a second program (or edit the CAM-generated program) to include tapping subroutines.

This is example of what sprut posts long hand setting. No settings on the feed , speed, pitch
I did set a put in .3 pause at bottom of cycle.

N10 G90 G64 G50 G54 G80 G17 G40 G49
N20 G20 (Inch)
(Hole Tapping)
N30 M998
N40 T52 G43 H52 M6
(tap)
N50 S500 M3
N60 G0 G94 X2.5 Y-2.
N70 Z0.3937
N80 (Hole93)
N90 Z0.0394
N100 G1 Z-0.52 F12700
N110 M4
N120 G4 P0.3
N130 Z0.0394
N140 G0 Z0.3937
N150 M3
N160 G4 P0.6
N170 M5
N180 M998
N190 M30



Example of canned post from sprut

N10 G90 G64 G50 G54 G80 G17 G40 G49
N20 G20 (Inch)
(Hole Tapping)
N30 M998
N40 T52 G43 H52 M6
(tap)
N50 S500 M3
N60 G0 G94 X2.5 Y-2.
N70 Z0.3937
N80 (Hole93)
N90 S500 M3
N100 G1 Z-0.52 F19.7
N110 M4
N120 G4 P0.3
N130 G1 Z0.0394 F15
N140 M3
N150 G4 P0.
N160 G0 X2. Z0.3937
N170 M5
N180 M998
N190 M30


There is about 2 dozen more settings and tap configurations in sprut
I see one thing strange with the posts above ... anyway
I have a couple of fixture plates on the drawing board that will require me to tune this process by testing.


md

[TurboStep]

There's a strange mix of dimensions inch + metric converted to inch which doesn't make it any easier to follow. The feed rate conversion went the wrong way in the first example - I hope that Sprut didn't do that!
Step

[mountaindew]

There's a strange mix of dimensions inch + metric converted to inch which doesn't make it any easier to follow. The feed rate conversion went the wrong way in the first example - I hope that Sprut didn't do that!
Step

Both were generated by sprut.
Please explain what mix I see g20 but no other metric/ inch reference ?
md

[TurboStep]

Both were generated by sprut.
Please explain what mix I see g20 but no other metric/ inch reference ?
md

Sorry for not being very clear. I was just referring to values like Z0.3937 which equates to 10.00mm. This is ok, but the feed rates seem to be a bit messed up. In the first example the value looks like 500mm/min converted to inches, but in the wrong direction i.e. 500*25.4=12700. Dividing 500 by 25.4 gives 19.685, or approximately the first feed rate in the second example on line N100. If the only difference between the first and second examples was changing the long hand to the canned setting then Sprut really messed up!
Step

[mountaindew]

Sorry for not being very clear. I was just referring to values like Z0.3937 which equates to 10.00mm. This is ok, but the feed rates seem to be a bit messed up. In the first example the value looks like 500mm/min converted to inches, but in the wrong direction i.e. 500*25.4=12700. Dividing 500 by 25.4 gives 19.685, or approximately the first feed rate in the second example on line N100. If the only difference between the first and second examples was changing the long hand to the canned setting then Sprut really messed up!
Step

oh, sorry sprut has so many default values for safe this and move that and I had no idea where it come up with them until now. All those funny numbers are conversions to inch
In general I change all those numbers to values that I like to see in code but had not used this enough to set defaults for each safe plane ....................................whatever setting.
And agreed the f12700 number was first thing my eye went to.

Thanks for pointing out that all those defaults are metric converts.
That explains so much in my little world of software design and programing standards.

I looked at other tap code examples and both looked correct and both would work . The added pause command being the difference I see.
A did test run the 1st example . Drilling 98 holes and then it simulated the tap operation by using same tool and letting it run 98 tap cycles in 6x5x3/8 acrylic.
I don't have a tc unit until later this week. Then I can do a full test, setup and get it tuned well enough to setup defaults in sprut .

Turbo what else should sprut have generated long hand cycle?
It looks like code H. posted a couple pages back to me .
Thanks for help and input
md

[mountaindew]

Just to follow up on my experience with tapping using tc unit and 8-32 spiral taps
The long hand generated by sprut did not work correct with my settings.

The Tap cycle with the canned post selection set with 500 rpm, cut speed set to 15.62 per formula, A .04 pause and .0312 pitch worked for 93 tapped holes in a row.
Also it worked best if you set the Safe distance to like 0.2 and not the .03 it defaults to.
The tap is not always fully retracted before it wants to take off to next location. Easy to see this should be set to a larger number because the tc unit has more tool travel then the default value by 10 times.
Anyway this was worked out good overall for 1st test and experience with cnc tensions compression tapping units

.
Example of canned post from sprut


N10 G90 G64 G50 G54 G80 G17 G40 G49
N20 G20 (Inch)
(Hole Tapping)
N30 M998
N40 T52 G43 H52 M6
(8-32 tap)
N50 S500 M3
N60 G0 G94 X2.5 Y-2.
N70 Z0.5
N80 (Hole93)
N90 S500 M3
N100 G1 Z-0.34 F15.6
N110 M4
N120 G4 P0.4
N130 G1 Z0.25 F15.6
N140 M3
N150 G4 P0.
N160 M5
N170 M998
N180 M30

I cut code for all the holes and pasted only the 1st one in the example above for easy reading.
hope this helps !