Tapping Code Output

[Post dept]

Does anyone actually want the M03 output before the M29 for rigid tapping?

 

This is an mpmaster thing that has been around for a while. I find that most people want it removed.

 

Let me know what you guys want and I'll change it if required.

 

Brett

[Columbo™]

This is what I output

 

 

N1130T70

N1140M06(1/4-28 RIGID TAP)

N1150G90G00G54.1P2X0.Y-.44A90.S280M03

N1160G43H70Z5.M08

N1170G95

N1180M29S280

N1190G84G98Z.9R1.5F0.0357

N1200G00G80Z10.M09

N1210G94

N1220G91G00G30Z0M05

N1230M09

N1240G28X0Y0

N1250G90G00A90.

 

 

[Post dept]

You use the M03. Controller? Ever tried without it?

[Columbo™]

No I haven't, why?

 

What would happen?

[doyleg]

I think that it should probably stay in as it is. I once had a prob when the rpm was programmed wrong. It was supposed to be s500 but came out as s5000. I was just beginning at the time and didn't notice the higher rpm. While in machine putting moly-dee on part the machine took off like a bat out of hell and drove straight down through the part and into the table. The printout of the code said s500 so i figured it was good. After cleaning my drawers i reran at +5. in z, single block, and it still hit the table. I finally backed off and took some time to calm down and reran it again. This time I hit cycle start and immediately heard the spindle wind up and realized it was the spindle speed that was wrong. It is now "One" of those things that will never happen again. (and after 18 years it hasn't)

Just one case as to why it should stay.

[Matt Sumner]

Outputting tapping with no M03 on most controls will cause the spindle to run only during the tapping of the hole. With the M03 the spindle turns on and off when moving from one hole to the next. On certain machines this can add a lot of time especially if there are a lot of holes to be tapped. If this adds 2 seconds per hole on a run of 2000 parts each having 20 holes you will be adding 22 hours to the run time.

 

Seems like free money to me.

[Post dept]

Does our accounting dept have any openings?

[Keith @ Solid Code Solutions]

quote:

---

Outputting tapping with no M03 on most controls will cause the spindle to run only during the tapping of the hole

---

Doesn't this really only apply to the first hole as there will be stops prior to feed for orientation, and then change of direction to feed out then stop at feed/clearence plane then position for hole two and so on.....

 

I still have the M3 in my post output mind you.

 

quote:

---

(PROG: A)

(DATE: 07-24-07)

(TIME: 15:02)

(NC FILE - Z:OKUMA3A.MIN)

(MATERIAL - STEEL INCH - 440 STAINLESS - 400 BHN)

(POST NAME - ITD_Okuma)

(****TOOL LIST****)

(T12| 5/16-18 TAPRH |H12|D12|Dia .3125" )

VTOFD[12 ]=0

(****PROGRAM START****)

G90

G15H1

G0 Z30

VMPC2=1

VMPT=0

(PROGRAM MAX: Z1.")

(PROGRAM MIN: Z-.5027")

N12

M1

(TAP_VENT PINS)

(T12| 5/16-18 TAPRH |H12|D12|Dia .3125" )

(OPERATION MAX: Z= 1.")

(OPERATION MIN: Z= -.5027")

/ T12 M6

G0 G90 X-3.1031 Y1.8018 S180 M3

G94 G56 H12 Z1.

Z.05

G284 Z-.5027 R.05 F10. S180 M54

X-1.1011

X1.1011

X3.1031

X-3.1031 Y-1.8018

X-1.1011

X1.1011

X3.1031

G0

Z1.

G0 Z18.

Y18

M30

%

---

[?Mark]

quote:

---

I find that most people want it removed.

---

Same here. No need for M3 when using M29 for rigid tapping in our shop (fanucs only though).

All this code will do is rev up the spindle unnecessarily prior to tapping.

[3rdstring]

I say leave the M3 in.

 

I have a machine with a fanum 0 control that without that initail spindle call will sit at the intial plane and not rapid down to the r plane.

 

quote:

---

(#10-32 TAP)

N400M6T8

G54G0X#520Y0S200M3

M53

G4X1.

G43Z3.H8

M29S200

G95

N401G84G99Z-.47R.1F.0313

N402X#520Y1.625

N403X#520Y3.25

...

G98

N420X#521Y0

G80

M54

G94

---

[Guest CNC Apps Guy 1]

Ok, who's machine can tap at 5,000 RPM???

 

I leave it in and do not find any wasted time. Of course my machines can achieve Max RPM in less than 3 sec for the most part. The 24k spindle takes a bit longer, but not much.

 

I also leave it in because some machine automatically change gaear according to spindle speed, so the initial speed call gets the gear right, then it's set to rigid tap. Granted it only saves a few sec per cycle (not per hole), yeah I suppose it could add up over the course of a year.

 

SOmething else I do is put in an M19 before the rigid tap call, this allows me to go into the same hole provided I have not changed the retract height or the height offset for the tap.

 

JM2C

[DavidB]

James,

I didn't think the M19 was needed to run down the same hole twice.

I dont use M19 in my posted code but I have re run the tap down, like you said as long as the retrcat heights have not changed.

 

[Post dept]

Huh, looks like we're all in agreement eh?

 

Maybe I'll rough in the logic to leave out the M03 but leave the M03 output as the default.

 

Look for a big Mpmaster update soon.

[Post dept]

After further thought, how about a switch called rigid_tap that suppresses speed and spindle call then gives M29 output before tapping?

 

This would work the same way as mplmaster.

[Tim Johnson]

quote:

---

Ok, who's machine can tap at 5,000 RPM???

---

The smaller Enshus will tap at 6000 rpm. We tap at 4000 rpm every day (larger Enshus).

[gms1]

Our rigid tapping cycles look like this

 

G0G90G54X-1.Y-1.T2

G43H1Z.1

M8

M29S200

G98G54Z-1.F20.

X-5.

X-7.

G80M9

 

I had my old V9 post setup with a misc. int. to turn off the spindle speed command on the start of the canned cycle line when I was tapping. For my Vx+ posts I just didnt bother and left the speed command in the top line. It would be great if we could get that removed from the 1st line of the canned cycle because we never run the spindle inbetween holes. It just takes to long on some of our old and slow machines.

[Guest CNC Apps Guy 1]

Rigid @ 6,000 - WOW! Very impressive.

 

Can you do a 1"-8 that fast

 

Sounds cool Brett!!!

 

Once again, you da man!!!