G76 Threading cycle

There appear to be several version of the G76 threading cycle.

In the Linux cycle the parameters are P,Z,I,J,K,R,E,L Where P is the pitch and I is the thread peak offset from the drive line

Yet in other versions I have read that P is a 6 digit number and F is the pitch .

Does Linuxcnc use a none standard version.

I am on a steep learning curve and getting confused (probably my age)

This is what I have used to try and cut a 10mm x 1.5mm pitch thread.

G7
G0 X10 Z2
G76 P 1.5 Z-10 I -0.1 J 0.1 R1.0 K 0.92 Q0 H2 L1
G0 Z0
G0 X40

I am touching off at X0 centre and Z0 end of bar.

Am I doing this correct? Do I have the parameters and numbers correct for G7 Dia mode.

Thanks Clive

Hi

Yet in other versions I have read that P is a 6 digit number and F is the pitch .
Does Linuxcnc use a none standard version.

Every controller varies, the only thing you should be reading is the documentation for linuxcnc.

I posted this recently for another user, hopefully will be of use to you too.

www.linuxcnc.org/index.php/english/forum...lem-stepconfig#57063

regards

ArcEye wrote:

Hi

Yet in other versions I have read that P is a 6 digit number and F is the pitch .
Does Linuxcnc use a none standard version.

Every controller varies, the only thing you should be reading is the documentation for linuxcnc.

I posted this recently for another user, hopefully will be of use to you too.

www.linuxcnc.org/index.php/english/forum...lem-stepconfig#57063

regards

Thanks. I think you did post this to me in another thread. I found it very useful.

I think it may have dawned on me after I have re read your post. In that Ihave used 0.92 for the K peram. should that have been doubled because we are in G7 Dia mode?

I have been going round in circles reading all the stuff I could find re G76 and getting nowhere.

Clive

Thanks. I think you did post this to me in another thread.

Should have noticed that, sorry

I always program in diameter mode, since the finished diameter is what you measure, so never really had the confusion regards radius.

If you look at the example I gave, I just used 1.5mm for both P and K, since a metric standard 1.5mm thread is equal in depth and pitch.

So yes, the total depth is 3mm, ie 3mm lesser diameter than the peak of the thread, but the depth of cut is 1.5mm.
Clear as mud!

Basically you program in the dimensions of the thread, not the overall dimensions of the billet with the thread cut into it.

regards

Thank you Sir ArcEye.

I have now successfully cut my first cnc thread 10mm on my little ML-S7 lathe cut the encoder disc on the router Index A & B 64 slot.
With the help on here I have got the hal files sorted etc

It was the dia mode G7 that fooled me the most and the different flavours of G76.

Clive

www.cncknowledge.in/2018/07/g76-fanuc-th...ith-description.html
N10 M06 T01 01 ;
N20 M04 G97 S1000 ;
N30 G00 X45 Z5 ;
N40 G76 P020060 Q100 R50 ;
N50 G76 X38.7 Z-50 P1227 Q100 F2 ;
N60 G00 X45 Z5 ;
N70 M05 M09 M30 ;

DESCRIPTION OF MAIN PROGRAM :-

N10- Tool change command , select tool no. 1
N20- Spindle ON anti clockwise , constant spindle speed command , speed is 1000 rpm
N30- Rapid action command where X45 and Z5 .
N40- Threading cycle command , P020060
( P02 = No. of finished path
00 = Chamfer amount at end
60 = Angle of tool tip ) ,
Q100 = Each cut is 0.1 mm ,
R20 = finishing allowance 0.02mm
N50- Threading cycle command , Minor dia X axis , threading along Z- axis up to -50 , Threading depth , Depth of finish cut 0.1 mm , pitch is 2 .

: M40X2

Major diameter is 40
Pitch is 2
Thread depth calculation = Pitch x 0.61363
= 2 x 0.61363
= 1.227 mm in micron is 1227

Minor diameter = 40-1.23 = 38.7 mm

N60- Rapid action command where X45 and Z5 .
N70- Spindle off , coolant off , main program end .
for more info visit- www.cncknowledge.in

I am not sure that flavour of G76 is the same version in Linuxcnc