Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
Percentage of people using G-code system A, B and C
- Thread starter sinha
- Start date
- Replies 34
- Views 12,832
Vancbiker
Diamond
- Joined
- Jan 5, 2014
- Location
- Vancouver, WA. USA
In the better part of 40 years of being around CNC machines, I think I have only seen one or two that used B or C.
alphonso
Titanium
- Joined
- Feb 15, 2006
- Location
- Republic of Texas
I've got an 0TC that use system B. My 0m-Mate and 18MC use whatever the hell is in the manual, probably system A.
alphonso
Titanium
- Joined
- Feb 15, 2006
- Location
- Republic of Texas
Now you are confusing me. Both the 0m-mate and 18mc use G28 X.Y, Z. So what system do I have?
A, B, C apply to lathe only.
mikiemus
Aluminum
- Joined
- Sep 23, 2012
- Location
- Sweden Malmoe
@ Europe:
A versions are most common, what I know.
B versions for e.g. Lathes with Live tools. e.g. Fanuc -TB
C versions, never seen in a machine shop, but we use it at our school. (duh)
Difference of Lathe A and B version is G98, G99. A-version lacks it.
The C-version we use at school, might just be for the Emco switchable control ability,
or just their 'fancy' way of design. Im used to A and B, so C is just confusing.
So, those Fanucs that I encountered, are 65% A, and 35% B.
mikiemus
Aluminum
- Joined
- Sep 23, 2012
- Location
- Sweden Malmoe
While our Lathe Fanuc 21, with C-list, performs G28 U0 perfectly. (G28 X0 makes it go X0, then X-home. like double move)
(parameter settings could fool anyone, to be too certain)
gregormarwick
Diamond
- Joined
- Feb 7, 2007
- Location
- Aberdeen, UK
You are confusing control revisions with the g-code system.
mikiemus
Aluminum
- Joined
- Sep 23, 2012
- Location
- Sweden Malmoe
Not talking about revisions. G-code list. Its a parameter setting in Fanuc.
angelw
Diamond
- Joined
- Sep 10, 2010
- Location
- Victoria Australia
Hello mikiemus,While our Lathe Fanuc 21, with C-list, performs G28 U0 perfectly. (G28 X0 makes it go X0, then X-home. like double move)
(parameter settings could fool anyone, to be too certain)
I would be very surprised if that is the case, as selection of Absolute/Incremental by G90/G91 respectively is one of the aspects that sets G Code Systems B and C apart from System A. I've not seen a case where Incremental or Absolute commands can be executed by both G90/G91 and XZ/UW respectively in a Fanuc control set to use either G Code System B or C.
System A has G98/G99 commands; they just differ in there use to that of System B and C.
Because Fanuc controls are supplied to a wide range of MTBs, according to my Fanuc Colleagues, System B and C are provided to give comparability with other controls. Also, when System A is used, U, V, or W can't be used as an axis name. Accordingly, G code system B or C is used for multi axis Turning Centres.
Regards,
Bill
gregormarwick
Diamond
- Joined
- Feb 7, 2007
- Location
- Aberdeen, UK
The letter suffix on the control type is the control revision, not related to the g code system used on the control.
mikiemus
Aluminum
- Joined
- Sep 23, 2012
- Location
- Sweden Malmoe
Ahh, -TB, yes. lol
I think this is the answer to my query.
With live tools, the final retraction in drilling/tapping cycles would be up to the R-point or the initial level depending on G99/G98, in G-code system B and C.
System A uses G98/G99 for a different purpose (feed per minute and feed per revolution, respectively).
Final retraction in system A is parameter dependent:
5161#1 = 0 causes initial level retraction
5161#1 = 1 causes R-point retraction
So, there is no limitation in system A.
mikiemus
Aluminum
- Joined
- Sep 23, 2012
- Location
- Sweden Malmoe
This confuses me a bit. I have run Fanuc 0T with system A and I can use X,Z as absolute and U,W as incremental full free, and mix them as I like. e.g. G0 X100 W-10 Works fine. All our OT System A, was like this.
If you want to be surprised I can show you a movie from a system C machine there I (in MDI) perform G21 (thread cutting cycle) in absolute programming and immediately after just type G28 U0 W0 for running to home position. What I want to say by this is following... Not all controls are setup parameterwise as we would expect. Have to learn the individual control at spot, due no one can ever know what settings it has. Ususally workers are there to make pieces and digging in parameters is not what a shopowner expects from a worker.
Page of manual:
View attachment Lathe.pdf
Cheers,
Mikie
