[Kai_DK]

Hi.
When threading, I use G76.
I know of 2 ways to descripe the syntax for the thread, but I can only find the right syntax for single line G76.
I have G76 X8. Z-10. P613 Q250 F1 A60 for an internal M8*1 thread.
I would like to try to use the dual-line G76, but whats the syntax?
I need it to be able to switch between ways to execute the way the thread is made (front of insert, back of insert, etc.)

[cogsman1]

G76- Canned threading cycle

G76 P010010 Q0020 R0005 (first G76 sets parameters for threading)
G76 X Z P Q F R (cuts the thread)

The first G76 isn't needed but is recommended.
- G76 P Q R

P010010 sets 3 things
- first 2 digits is the amount of finish passes - 01

- second 2 digits is % of the lead or pullout exiting the thread- 00
00 = almost no angle at pullout and 99 = 9.9 leads away start out

- third 2 digits are the angle of infeed - 10
0-99 are usable

Q0020 sets the minimum cut amount during threading .002 but no decimal
(Q00200 for sub inch)

R0005 sets the cut amount of the last pass .0005 but no decimal
(R00050 for sub inch)

The second G76 cuts the thread.
-G76 X.1876 Z.3 P0302 Q0010 F.05 (R-.002) FOR 1/4-20

X.1876 =Minor Dia. of thread

Z.3 or (W) =The ending Z of the thread

P0302 =Height of thread in radius (Maj-Min)/2 (.0302)
(P03020 for sub inch)

Q0100 =Amount of the first cut. All the rest of the cuts are calculated.
(.01)
(Q01000 for sub inch)

F.05 =Feed-rate 20 TPI 1/20=.05

R = R is optional for tapered threading. R is the amount of
difference in X from start to finish in Z. When cutting threads
moving Z and X in a positive direction R is a negative value.

[Karl_T]

Great info here, in a better format than I've come accross.

I'm programming my <Camsoft> lathe to do G76.

I have a question on Z start. Will the control always start threading at the current Z position and then go to Z end speced in G76 line 2? Or will it error if you're too far away? In other words, how does the control know how long the threading pass is?

Second, left hand threads. Do you just use all negative values and cut on the backside of your part?

Karl

[cnc-king]

Great info here, in a better format than I've come accross.

I'm programming my <Camsoft> lathe to do G76.

I have a question on Z start. Will the control always start threading at the current Z position and then go to Z end speced in G76 line 2? Or will it error if you're too far away? In other words, how does the control know how long the threading pass is?

Second, left hand threads. Do you just use all negative values and cut on the backside of your part?

Karl

i always set my z to start 1.5 turns from start of threads
for left hand threads i use a holder that will accomadate both left and right thread inserts and all i have to do is reverse the spindle

referring to cogsman the last 2 digits in the first g76 line is determined by the angle of your threads which is normally 1/2 of the included angle of the thread

[Kai_DK]

...but how about the option of theading with the front or the back of your insert?
BTW, thank you for info.

[M-man]

If you have the F10TA/F11TA you use P1 for one-side, constant cutting amount
P2 zigzag with constand cutting amount
p3 and p4 just like p1 and p2 but with constant cutting depth.

for the F0TA I dont think you can apply type of cutting, but if you got special threading needs, use G32.

G76 X27.4 Z-52 K1.3 D400 F2. A60 P1 --- F10TA style

G76 P011060 Q50 R50
G76 X27.4 Z-53 P1200 Q400 F2.0 --- F0TA style

[g-codeguy]

Great info here, in a better format than I've come accross.

I'm programming my <Camsoft> lathe to do G76.

I have a question on Z start. Will the control always start threading at the current Z position and then go to Z end speced in G76 line 2? Or will it error if you're too far away? In other words, how does the control know how long the threading pass is?

Second, left hand threads. Do you just use all negative values and cut on the backside of your part?

Karl

You program both the Z-axis start and finish positions. Machine threads between these 2 dimensions (minus compound infeed). One manual suggests 3 times the lead or .3 whichever is greater. At high RPM I usually start .5 in front of the thread. This is to allow the machine to accelerate to the correct feed. Machine will not error out because of thread length.

Do not change start position, RPM, or compound infeed if re-threading. It will cause a double thread. Compound infeed on the 2-block G76 call is not adjustible from 0-99. At least not on the lathes I run. You are allowed 6 options: 0, 29, 30, 55, 60, or 80. The single block call has an A-value for the compond infeed which allows you to use any number between 0-99.

For left hand threads, follow the advice already given. Use a left hand threading tool and reverse the spindle direction.

Kai_DK asked about cutting with both sides of the tool. M-man's answer was correct. Notice that this option is only available in the single block call.

You control (somewhat) how much the insert cuts on a side by using the compound infeed function of the last pair of values in the P word in the first block. 0 (zero) value has no compund infeed and cuts equally on both sides of the insert. This is a tough chip. Only used it once in 22 years of programming. 60 cuts only on the leading edge (for standard 60 deg. threads). This creates less tool pressure if you are having a chatter problem. Not the best for use on work hardening materials. Normally I stick with 29 or 55. Q in first block is minimum DOC. R is DOC of last pass. On work hardening materials you will need to keep a large enough value to make a decent cut if possible.

As stated, the middle 2 values in the P word in the first block is for pull out. 00 will leave a ring on the last thread. I only use it with threads having a relief. I use 01 otherwise so the machine will pull out as quick as possible. Often I am threading to a shoulder and need to get as close as possible.

Speaking of getting close to a shoulder, slow the RPM down if the 01 value won't get close enough. The slower RPM allows the insert to stay in the cut for longer. Not always best for the insert because it will be below its best operating range, but sometimes necessary.

Hope this was of some help to you.

[M-man]

I always use a m-code to decide if there are chamfer or not at the end of thread, threads I make with P010060 makes a nice way out at the end even thou there shouldnt be any chamfer, mabe there are a parameter set for this amount if it is EQ to zero???. With the m-code I can make the right pitch closer to the shoulder.

And there are actual formulas to calculate the exact amount of start and end distance of the acceleration of servo when threading at certain spindle speed.

[habertt]

I have been having a problem with my thread getting a taper and causing issues with plating. The diameter is .003 smaller at z-1.735. I have made it, overall,.004 smaller but can't get rid of the taper. How do I do it. Here's my cycle for a 1/2-20 thread. (Mori ZL25-B500, Fanuc MF-D6 (16TTA) control)

G76 P040060
G76 X.4392 Z-1.735 P0500 Q0100 F.05

[Karl_T]

I have been having a problem with my thread getting a taper and causing issues with plating. The diameter is .003 smaller at z-1.735. I have made it, overall,.004 smaller but can't get rid of the taper. How do I do it. Here's my cycle for a 1/2-20 thread. (Mori ZL25-B500, Fanuc MF-D6 (16TTA) control)

G76 P040060
G76 X.4392 Z-1.735 P0500 Q0100 F.05

Try adding an R.003 to your second line. Should correct for your taper. You may have to experiment with the value for your control.

Karl

[g-codeguy]

Try adding an R.003 to your second line. Should correct for your taper. You may have to experiment with the value for your control.

Karl

On our machines, this would make the taper worse. The X value in the threading cycle would be at the Z-1.735. A value of R.003 would increase the root diameter by .006 at the front of the part. (Maybe not exactly .006 because of tool pressure.) Check the manual for your machine to see how the R-value works for it.

Karl is correct when he stated that you may have to experiment with this value. Just because it is mathematically correct doesn't mean it will work out. I usually find I have to go more than what the taper is...depending on the material and size of the tool.

[cogsman1]

I have been having a problem with my thread getting a taper and causing issues with plating. The diameter is .003 smaller at z-1.735. I have made it, overall,.004 smaller but can't get rid of the taper. How do I do it. Here's my cycle for a 1/2-20 thread. (Mori ZL25-B500, Fanuc MF-D6 (16TTA) control)

G76 P040060
G76 X.4392 Z-1.735 P0500 Q0100 F.05

Add "R-.004" on second G76 line to cut .004 taper.

G76 P040060
G76X.4392Z-1.735P0500Q.010F.05R-0.004

[sinha_nsit]

Add "R-.004" on second G76 line to cut .004 taper.

G76 P040060
G76X.4392Z-1.735P0500Q.010F.05R-0.004

This should work. If the meaning of R (e.g., its sign) is causing any confusion, remember that it is exactly same as R of G90 (Somebody correct me if I am wrong. Actually, I have done a lot of thinking on it and came to this conclusion).

Some clearance at the start of thread (3-4 leads) is recommended, because otherwise the start of the thread might have incorrect lead due to a possible lag is the servo system.

There is one more comment:
Choose any RPM. The machine will automatically adjust the feed to suit your thread lead (lead = pitch x no. of starts of the thread), provided the required feed is not higher than the maximum possible feed on your machine. If this is indeed the case, reduce RPM suitably, because otherwise the machine will only move as fast as it can, without giving any error message.

[habertt]

Thanks! I'll give it a try.

[harshal]

Fanuc g32 threading cycle program II Single point threading II
August 01, 2018 - FANUC G32 THREADING CYCLE [T]



- angle -
Click Here to Continue to angle
O1571
N10 M06 T02 02 ;
N20 G50 S1500 ;
N30 M03 G97 S200 ;
N40 M08 ;
N50 G00 X30 Z3 ;
N60 G32 X29.08 Z-50 F1.5 ;
N70 X28.78 ;
N80 X28.48 ;
N90 X28.18 ;
N100 G28 U0 W0 ;
N110 M05 M09 M30 ;
More examples..........!!!!
DESCRIPTION OF MAIN PROGRAM :-
Calculation :- Depth of thread = 0.6134 X Pitch
= 0.9201
Crest = major dia - 0.9201
= 29.08
Root = Major dia - 2 x Depth of thread
= 30 - 2 x 0.9201
= 28.16 (root)
Each cut is 150 microns =0.15mm , it means total reduce 0.30 mm and cutting upto root 48.16 mm
First cut is 29.07 mm (Crest)
Second cut is 29.07-0.3 = 28.78
Third cut is 28.78-0.3 = 28.48
Final cut is 28.48 -0.3 = 28.18 (~ 28.16)(root)
*************************all dimension in mm ***********************************
01571 - Name of main program
N10- Tool change command , select tool no 2
N20- Maximum spindle speed command , speed is 1500 rpm
N30- Spindle ON clockwise , constant spindle speed , speed is 200 rpm
N40- Coolant ON
N50- Rapid action command , where X30 and Z3 .
N60- Threading cycle command , where X29.08( crest )(First cut) and Z-50 , feed rate is 1.5 ( it is always is equal to pitch )
N70- Second cut is 28.78 in X axis
N80- Third cut is 28.48 in X axis
N90 - Final cut is 28.18 in X axis (root)
N100 - Reference position command , where X0 and Z0 ;
N110 - Spindle OFF , coolant OFF , main prog. end

my link is
CNC PROGRAMMING TUTORIAL

[angelw]

Fanuc g32 threading cycle program II Single point threading II
August 01, 2018 - FANUC G32 THREADING CYCLE [T]

- angle -
Click Here to Continue to angle
O1571
N10 M06 T02 02 ;
N20 G50 S1500 ;
N30 M03 G97 S200 ;
N40 M08 ;
N50 G00 X30 Z3 ;
N60 G32 X29.08 Z-50 F1.5 ;
N70 X28.78 ;
N80 X28.48 ;
N90 X28.18 ;
N100 G28 U0 W0 ;
N110 M05 M09 M30 ;

You keep dredging up these ancient Thread to promote your own web site, giving the impression that you're some kind of expert; then you spoil the illusion by Posting an example that puts on show your lack of programming knowledge. When using G32/G33 Threading Function, you have to:

1. Locate the tool at the X/Z Start coordinates
2. Locate the tool at the X (longitudinal threading) cut diameter
3. Execute the Threading Pass with G32/G33 and a Feed Rate
4, Withdraw the tool from the cut to clear the Thread
5. Return the tool to the Z Start coordinate
6. Repeat steps 2 to 5 until the Thread is cut to full depth

You can't simply specify the next X diameter as you have in your example; accordingly, your program will fail. Being able to specify each successive X value is in the realm of the G92/G78/G21 (depending on the G Code System the Machine uses) Threading Cycle.

Frankly, the erroneous nature of your Posts puts me off visiting your web site.