Hey Zolko, great to have a contributor like you come visit here
G54 is typically what the CNC nomenclature call a Work Coordinate Offset (or variations thereof depending on the ISO or other norm).
Typically any machine will use offsets G54 to G59. So G54 is considered the "default" one. Often also the pivot point of a 5 axis platform. Note that G53 is absolute machine coordinates and usually follows it's own rules (such as, G53 must be specified for each line of movement code if one wants to use this reference).
They behave very much like the machine version of a Local Coordinate System which you know very well
G54-59 are modals. This means if read once in the code, the whole following code will stay in this reference system.
Hence when your code says G54 at the start, this means all G01 and G02/G03 codes (linear and arc interpolation) will be executed based on that reference.
But it means you must set G54 first on your workpiece. That's usually when you touch off your part using a probe or dial indicator or the tip of your tool...and set the reference. Usually if your machine interface says "set reference" without specifying, it is G54. But you must check.
In the virtual world of Path Workbench, when you create a job the Coordinate System Reference you see displayed is going to be your G54. Path creators and contributors made the tool easy to use and you can select a vertex and apply the reference, orient it..etc. Refer to Sliptonic's great suite of instructional videos on Youtube.
What happened in your case is what chrisb said. You created two jobs, with two slightly different virtual stocks. Hence two slightly different references. So executing both codes means each is referring to another slightly shifted G54, but your machine had only one G54 set for all your operations.
ProTip: if you want to set G54 where your machine is currently you can send the code G92G54X0Y0Z0
Which says "please reset position of G54 at 0;0;0"
Hope this helps, happy chipping!
G54 and fixtures
Forum rules
Be nice to others! Respect the FreeCAD code of conduct!
Be nice to others! Respect the FreeCAD code of conduct!
-
- Posts: 991
- Joined: Wed Mar 27, 2019 10:45 am
Re: G54 and fixtures
Thank-you for your explanation. So G54 is the default coordinate system, the "LCS_0" of a Path Job, if nothing else is set, if I understand correctly. It is possible to set other coordinate systems, but if not G54 is the one in use.RatonLaveur wrote: ↑Sun Dec 08, 2019 7:09 pm In the virtual world of Path Workbench, when you create a job the Coordinate System Reference you see displayed is going to be your G54.
Re: G54 and fixtures
Hi Zolko,
yes it is.
At LinuxCNC homepage is a explanation about the G- and M Codes
http://linuxcnc.org/docs/2.7/html/gcode/g-code.html
yes it is.
At LinuxCNC homepage is a explanation about the G- and M Codes
http://linuxcnc.org/docs/2.7/html/gcode/g-code.html
Gruß Herbert
Re: G54 and fixtures
I think G53 is the CS which is used if noone is explicitely set, not G54??
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
- sliptonic
- Veteran
- Posts: 3457
- Joined: Tue Oct 25, 2011 10:46 pm
- Location: Columbia, Missouri
- Contact:
Re: G54 and fixtures
Almost. G53 is the absolute machine coordinate system. G54 is the default system used.
-
- Posts: 991
- Joined: Wed Mar 27, 2019 10:45 am
Re: G54 and fixtures
It really depends on your type of CNC and how you configured it.
All the industrial CNC i've used work in a way that by default if you write:
G90
G53G01X10
G01X20
Then the machine will first move to the position X 10 in machine coordinates (which depending how the machine manufacturer configured G53, may be outside the work volume and will generate a hard stop or a spindle crash, since some machine standards specify G53 at the rear top right end).
Then it will automatically move to X 20 mm in G54.
If I wanted to go first to 10 and then 20 in the same G53 machine coordinates, i'd have to write:
G90
G53G01X10
G53G01X20
Just one of those things...check your CNC modal state (the current active modals) and see if G53 or G54 is active by default.
Hope this clarifies.
All the industrial CNC i've used work in a way that by default if you write:
G90
G53G01X10
G01X20
Then the machine will first move to the position X 10 in machine coordinates (which depending how the machine manufacturer configured G53, may be outside the work volume and will generate a hard stop or a spindle crash, since some machine standards specify G53 at the rear top right end).
Then it will automatically move to X 20 mm in G54.
If I wanted to go first to 10 and then 20 in the same G53 machine coordinates, i'd have to write:
G90
G53G01X10
G53G01X20
Just one of those things...check your CNC modal state (the current active modals) and see if G53 or G54 is active by default.
Hope this clarifies.