[jgarner77]

Hi guys i am having major trouble understanding how this clipping works,I've recently done 2 nut jobs with acme thread's and the customer insisted the front of the thread be backed off i was given the programs for these by the customer wich involves threading the part using G76 then running a sub program 8 times to the major diameter using G32 then tapering off in G32 when clearing the first thread.This works perfectly but i'd like to implement this into the other threads we do but i need guidance.I've read that in order for this to work the front of the thread tip has to be set on the same zero as the groove/turning tool i'm using to clip the thread i can't see how to achieve this as my turning tool is set on the front face of the part as zero but the threading tool is set at zero using the front of the tool and the actual cutting edge of the single point insert is set slightly back from that,can i just change the start position in z of the clipping passes to accomodate this difference also how do i work out how far to send my tool in z to clip the thread and at what angle should i program the G32 to angle out after clipping also one of the jobs i do it is imposibble to put a grooving tool into the setup as the turret is already rammed that is why i want to try and use a turning tool instead of a grooving tool to clip the thread

Thanks in advance for your replies i will try and post the program im using for the acme threads at the moment on monday as i forgot to bring the copy i made home

[txcncman]

You do not need G32. See example for using G76:

G80
G90
G00 G53 Z-18.
G00 G53 X0.
T404
G97 S150
G00 G54 X3.5 Z0.4 M03
G76 P2 X4.29 Z-1.493 D0.020 K0.1 A15 F0.1667
G76 P2 X4.166 Z-2.777 D0.020 K0.1 A15 F0.1667
G00 Z0.36
G76 P2 X4.29 Z-0.305 D0.040 K0.1 A15 F0.1667
G00 Z0.32
G76 P2 X4.29 Z-0.345 D0.040 K0.1 A15 F0.1667
G00 Z0.28
G76 P2 X4.29 Z-0.385 D0.040 K0.1 A15 F0.1667
G00 Z0.36
G76 P2 X4.166 Z-1.633 D0.040 K0.1 A15 F0.1667
G00 Z0.32
G76 P2 X4.166 Z-1.673 D0.040 K0.1 A15 F0.1667
G00 Z0.28
G76 P2 X4.166 Z-1.713 D0.040 K0.1 A15 F0.1667
G00 G53 Z-18. M09
G00 G53 X0. M05
M30

Note starting Z point and ending changes to allow for width of tool.

Also note, this is 2 different diameter, 6 pitch threads, each getting its own quick start.

[jgarner77]

Thanks for the reply txcncman i still don't understand how that works how would I go about clipping an m14 x 1.5 pitch external thread using a normal turning tool bearing in mind the tips of both inserts will be set at different zeros I just can't figure out how to get the turning tool in the same lead as the threading tool it was simple with the acme thread cause the insert is practically a grooveing tool and I use the same tool to thread and clip thanks again

[txcncman]

Assuming you will use a grooving tool for this. Also assuming you set the threading tool off the leading edge and not the tool tip. The start point and end point of the grooving tool will need to take into account the difference in the offset of the threading tool from its Z set point to the center of the tip. If the leading edge of the threading tool is 0.100" from the tip, allow for this 0.100" in the programming.

Does that help?

On the previous example, the threading tool includes a flat tip, so was used to also clip the thread. Could also be done for an acme thread, but not a V thread.

[jgarner77]

Thanks for the reply txcncman i still don't understand how that works how would I go about clipping an m14 x 1.5 pitch external thread using a normal turning tool bearing in mind the tips of both inserts will be set at different zeros I just can't figure out how to get the turning tool in the same lead as the threading tool it was simple with the acme thread cause the insert is practically a grooveing tool and I use the same tool to thread and clip thanks again

cant remember the exact program of the 2 G76 lines but its something like this
G00 X4.2 Z0.265T0909
G76 P020000 Q0050 R.0005
G76 X4.4 Z-2.0 P0100 Q0472 F0.3333(not entirely sure the info on these lines are correct with out looking at the program,i know the Z positions are right and think the X positions are somewhere near)


then the back off thread part of the program calls up T0909 again and brings it in too X4.24 Z0.4 then into the sub program 8 times to achieve the major diameter just clearing the first thread so:

G00 X4.24 Z0.4T0909
M98P80050

(sub program)
O0050
G00 U0.02
G32 Z-0.19
U-0.6W-0.4
G00 U-0.04
Z0.4
U0.04
U0.6
M99

Hope this helps or atleast you can try and give me some advice using G76 alone the control this is off is a fanuc 18t on an okuma and howa act-35 but most of the threads are done on fanuc 6t and 10t controls all on old mori seikis sl two's three's and four's

[jgarner77]

I understand that if setting the threading tool of the leading adge of the tool i need to make allowances for that as the centre of the cutting edge will be offset back from that but in my brief discussions with the cnc chargehand of the company i'm doing the acme threads for he said it was crucial that my tool always went back to the same place in Z before doing the next clip (in my case Z0.4) but your sample program shows it moving now i'm even more confused lol

[txcncman]

The flat on your tool for a 3 pitch Acme thread is 0.1236 I think. This means you will have to wipe out 0.3333 - 0.1236 of thread root, or 0.2097. I try to take less than 1/2 of the tool flat for each pass (0.1236 / 2 = 0.0618). So, you will need to adjust your Z start point and end point negative Z 0.0618 until the entire 0.2097 is covered. Also it is recommended to have 3 times the pitch as lead in for threading, I will change that below.

G00 X4.2 Z0.9999 T0909
G76 P020000 Q0050 R.0005
G76 X4.4 Z-2.0 P0100 Q0472 F0.3333

G00 Z0.8763
G76 P020000 Q0050 R.0005
G76 X4.4 Z-0.0618 P0400 Q0472 F0.3333

G00 Z0.8145
G76 P020000 Q0050 R.0005
G76 X4.4 Z-0.1236 P0400 Q0472 F0.3333

G00 Z0.7527
G76 P020000 Q0050 R.0005
G76 X4.4 Z-0.1854 P0400 Q0472 F0.3333

G00 Z0.9381
G76 P020000 Q0050 R.0005
G76 X4.4 Z-0.2472 P0400 Q0472 F0.3333

[txcncman]

I understand that if setting the threading tool of the leading adge of the tool i need to make allowances for that as the centre of the cutting edge will be offset back from that but in my brief discussions with the cnc chargehand of the company i'm doing the acme threads for he said it was crucial that my tool always went back to the same place in Z before doing the next clip (in my case Z0.4) but your sample program shows it moving now i'm even more confused lol

I am not sure where your chargehand gets his information. The example I gave is from a proven program. Starting at the same point makes the tool track the previously cut thread. I this case, we want to force the tool to "split" the thread (a little at a time). By moving the start Z point in, you are forcing this "split". There might be other ways to program this, but I have been doing it this way for years (since 1997).

[jgarner77]

I am not sure where your chargehand gets his information. The example I gave is from a proven program. Starting at the same point makes the tool track the previously cut thread. I this case, we want to force the tool to "split" the thread (a little at a time). By moving the start Z point in, you are forcing this "split". There might be other ways to program this, but I have been doing it this way for years (since 1997).

I'm not questioning your knowhow your far more experienced than me and the charge hand was from the company we are making the parts for and the programs were also proven and honestly up untill this point I've never really bothered taking the sharp edge of the threads we make we've just wire brushed them after they've been through the final op the method i posted works an absolute dream using the G76 followed by the G32 sub clipping program on the two nuts with the acme threads and I just want to try and implement some kind of clipping operation on the other parts we do to eliminate having to wirebrush them my main aim is to try and understand why and how to do it cause anybody can be given a copy of a program and make it work on a machine using the same tooling I'm just looking for some advice/guidance using either G76 or G32

Thanks again your advice is very much appreciated

[txcncman]

I was not discounting that you can use G32. I am saying this way is quick and easy. Just copy and paste the basic threading cycle and change a few numbers. With G32 it would look something like this:

G00 X4.2 Z0.9999 T0909
G76 P020000 Q0050 R.0005
G76 X4.4 Z-2.0 P0100 Q0472 F0.3333

G00 Z0.8763
G00 X4.4
G32 Z-0.0618 F0.3333

G00 X4.2
G00 Z0.8145
G00 X4.4
G32 Z-0.1236 F0.3333

G00 X4.2
G00 Z0.7527
G00 X4.4
G32 Z-0.1854 F0.3333

G00 X4.2
G00 Z0.9381
G00 X4.4
G32 Z-0.2472 F0.3333

Which will actually run even faster since is it not multi-pass threading. But, it will be harder on the tool and depending on material might leave more of a burr to be removed also.

[angelw]

G00 X4.24 Z0.4T0909
M98P80050

(sub program)
O0050
G00 U0.02
G32 Z-0.19
U-0.6W-0.4
G00 U-0.04
Z0.4
U0.04
U0.6
M99
Hope this helps or atleast you can try and give me some advice using G76 alone the control this is off is a fanuc 18t on an okuma and howa act-35 but most of the threads are done on fanuc 6t and 10t controls all on old mori seikis sl two's three's and four's

The Sub program works by gaining 0.02 in X every iteration of the Sub. Below is the resulting code expressed in Absolute, so you can see the tool path generated by the eight iterations of the Sub program. All modal addresses and axes moves have been included for clarity. You can achieve the same type of result by reversing the sign of the "U" moves for an external thread.

The Changehand statement is correct when using the listed Sub Program method and the fact that the thread being cut was an Acme, with a grooving tool being used to relieve the leading thread. If the Z start position is changed, then a slightly different thread start would be cut (as in multi start thread), resulting in the relieving tool gradually moving off of the crest of the thread along the Z axis.

Doing the same operation with a turning tool on a "V" form thread is a different kettle of fish. Because of the relatively small tool radius compared to the widest part of the thread form, formed by the "V" profile of the thread, you actually need the cycle to cut many multiple thread starts.

You wont be able to use the two block version of the G76 cycle with either the 6T or 10T control. These two controls use a single block version with the format as follows:


G76 X(U)_ Z(W)_ I_ K_ D_ A_ F_ P_

Where
X = Finish diameter of threading tool
Z = Finish Z point
I = Amount of thread taper expressed as radius from start point of tool.
K = Height of thread form expressed as radius
D = Depth of cut of first threading pass expressed as radius.
A = included angle of thread form
F = Lead of thread
P = Thread cutting method.

Regards,

Bill

(Pass #1)
G00 X4.2600 Z0.4000 (G00 U0.02)
G32 X4.2600 Z-0.1900 (G32 Z-0.19)
G32 X3.6600 Z-0.2300 (U-0.6W-0.4)
G00 X3.6200 Z-0.2300 (G00 U-0.04)
G00 X3.6200 Z0.4000 (Z0.4)
G00 X3.6600 Z0.4000 (U0.04)
G00 X4.2600 Z0.4000 (U0.6)
(Pass #2)
G00 X4.2800 Z0.4000
G32 X4.2800 Z-0.1900
G32 X3.6800 Z-0.2300
G00 X3.6400 Z-0.2300
G00 X3.6400 Z0.4000
G00 X3.6800 Z0.4000
G00 X4.2800 Z0.4000
(Pass #3)
G00 X4.3000 Z0.4000
G32 X4.3000 Z-0.1900
G32 X3.7000 Z-0.2300
G00 X3.6600 Z-0.2300
G00 X3.6600 Z0.4000
G00 X3.7000 Z0.4000
G00 X4.3000 Z0.4000
(Pass #4)
G00 X4.3200 Z0.4000
G32 X4.3200 Z-0.1900
G32 X3.7200 Z-0.2300
G00 X3.6800 Z-0.2300
G00 X3.6800 Z0.4000
G00 X3.7200 Z0.4000
G00 X4.3200 Z0.4000
(Pass #5)
G00 X4.3400 Z0.4000
G32 X4.3400 Z-0.1900
G32 X3.7400 Z-0.2300
G00 X3.7000 Z-0.2300
G00 X3.7000 Z0.4000
G00 X3.7400 Z0.4000
G00 X4.3400 Z0.4000
(Pass #6)
G00 X4.3600 Z0.4000
G32 X4.3600 Z-0.1900
G32 X3.7600 Z-0.2300
G00 X3.7200 Z-0.2300
G00 X3.7200 Z0.4000
G00 X3.7600 Z0.4000
G00 X4.3600 Z0.4000
(Pass #7)
G00 X4.3800 Z0.4000
G32 X4.3800 Z-0.1900
G32 X3.7800 Z-0.2300
G00 X3.7400 Z-0.2300
G00 X3.7400 Z0.4000
G00 X3.7800 Z0.4000
G00 X4.3800 Z0.4000
(Pass #8)
G00 X4.4000 Z0.4000
G32 X4.4000 Z-0.1900
G32 X3.8000 Z-0.2300
G00 X3.7600 Z-0.2300
G00 X3.7600 Z0.4000
G00 X3.8000 Z0.4000
G00 X4.4000 Z0.4000

[jgarner77]

thanks for your help guys very much appreciated and thanks for clarifying on which system uses the single line format and i take it that anything newer than a 10t control uses the 2 line format also sorry for the delay in getting back to you.I've been playing around with a few things at work and seemed to have cracked it whether its the right way or not it seems to work i can only assume that the reason the company we do the work for uses the G32 method is cause it allows you to control the angle at which the groove tool comes out at after clipping so doing a metric external thread on another machine (mori seiki with fanuc 10t) i just used a dnmg 0.4 radius style tip and programmed the tool to come 1mm further back than the threading tool (allowing for me setting the threading tool from the front of the holder and not the tip centre) so the tip of both inserts start in the same place and then programmed several passes using G92 to a depth of Z-2.1mm and to a diameter 0.001" below the minor diameter of the thread allowing the dnmg insert to clip the burr off as it pulls out it worked a dream and the tip starts and finishes in the same place in Z on every pass i'm sure i could've used G76 or G32 todo exactly the same but am so used to using G92

Thanks again guys for your help