Can't quite get to grasp with what the options mean and how it effect the thread...

K = 0: Flank in-feed constant volume removal for each pass

K = 1: Alternate flank in-feed constant volume removal for each pass

K = 2: Flank in-feed constant depth removal for each pass (each pass same as first pass)

K = 3: Alternate flank in-feed constant depth removal for each pass (each pass same as first pass)

Volume vs depth?

Could anyone explain please? I have read the manual, but the options seem to have an effect on the cut depth as well...

Right... found out the the manual says

K = 0: Flank in-feed constant volume removal for each pass

K = 1: Alternate flank in-feed constant volume removal for each pass

K = 2: Flank in-feed constant depth removal for each pass (each pass same as first pass)

K = 3: Alternate flank in-feed constant depth removal for each pass (each pass same as first pass)
but in reality its...

K = 1: Flank in-feed constant volume removal for each pass

K = 2: Alternate flank in-feed constant volume removal for each pass

K = 3: Flank in-feed constant depth removal for each pass (each pass same as first pass)

K = 4: Alternate flank in-feed constant depth removal for each pass (each pass same as first pass)
Jeez this Mach4 is hard work

Also doesn't help that when in Daimeter mode have the settings are in Diamter and the other half in Radius.

The G76 wizard is a bit of a mess really.

In most cases option 0 is the one to use.

Mach4 has two types of G76 try the Fanuc single line version its much less complicated. Page 46/47 in the lathe manual.

In most cases option 0 is the one to use.

Mach4 has two types of G76 try the Fanuc single line version its much less complicated. Page 46/47 in the lathe manual.

In most cases option 0 is the one to use.

Mach4 has two types of G76 try the Fanuc single line version its much less complicated. Page 46/47 in the lathe manual.

Thanks for the reply Graham. The single line is definitely easier.

One thing, the "Wizard" inserts a G99 into the code before the threading canned cycle. But the manual does not. Is the manual assuming you insert it or does the G76 automatically do it?

thanks again

Most lathes are run in feed per rev (G99) that way if you override the spindle speed the feed follows also G96 needs feed per rev to compensate for the change in diameter as the spindle changes speed so will the feed.

G98 & G99 are modal so if you do not change them they stay active so you normally have the G99 in your start up line.

Most lathes use feed rates between 0.05mm to 0.40 mm per rev for turning depending on the size and power of the spindle and the depth of cut.  When using carbide the speed and feed should be in the working range of the insert and the depth of cut adjusted to allow the machine to cut without issue.

If you are using CAM to program there will be an option for feed per rev (in fusion this is set in the tool library) or it may be a post option on some systems.

Its better to use feed per rev on lathes after all that is how a manual lathe works.

There is also the G32 and G92 threading options.

Most lathes are run in feed per rev (G99) that way if you override the spindle speed the feed follows also G96 needs feed per rev to compensate for the change in diameter as the spindle changes speed so will the feed.

G98 & G99 are modal so if you do not change them they stay active so you normally have the G99 in your start up line.

Most lathes use feed rates between 0.05mm to 0.40 mm per rev for turning depending on the size and power of the spindle and the depth of cut.  When using carbide the speed and feed should be in the working range of the insert and the depth of cut adjusted to allow the machine to cut without issue.

If you are using CAM to program there will be an option for feed per rev (in fusion this is set in the tool library) or it may be a post option on some systems.

Its better to use feed per rev on lathes after all that is how a manual lathe works.

There is also the G32 and G92 threading options.

Threading in Mach4 just seems so FLAKEY - you just cannot rely on it.

E.g. I can run a threading routine 10 times - no problem. Then I edit the Gcode to change a parameter in the G76 line and the next run the program hangs on the G76 line.

I have literally spent 4 days just trying to get the threading working. For a product that is supposed to be an "Upgrade" to Mach3 I feel a little bemused.

I also think they made the G76 threading too complicated for what is needed. In Mach3 you basically had an X starting point (Thread Major) a Z staring point. Then an X end point ( thread minor) and Z end point and pitch. Simple as you like. The "Ugrade" seems to be ironic in nature. E.g is it an "Upgrade" if you cannot reliably use it?

Use G92

%
G21 G00 G40 G99
G54
G00 X12. Z5. G97 S500 M3
G92 X9.8 Z-10. F1.5
X9.6
X9.4
X9.2
X9.
X8.8
X8.7
X8.6
X8.5
X8.45
X8.4
X8.37
X8.37
G80
G00 X120. Z120. M5
M30
%

Use G92

%
G21 G00 G40 G99
G54
G00 X12. Z5. G97 S500 M3
G92 X9.8 Z-10. F1.5
X9.6
X9.4
X9.2
X9.
X8.8
X8.7
X8.6
X8.5
X8.45
X8.4
X8.37
X8.37
G80
G00 X120. Z120. M5
M30
%

Tried this, worked lovely for 3 runs. The 4th run it locked at G92 line. 5th Run... it ran fine again. So I would say definitely an Index issue.

I did like the G92 code though, really nice and visible what's happening and really simple.

thank you

I have just checked the ESS docs,  are you powering the encoder from ESS port3 or is it from a separate 5V psu.

If from the ESS then try a separate PSU as the encoder may need more than the port can output.