Save table position

[Joostdmx]

Hi,

Is there a simple way to save a table x/y position in planet cnc?
Let me explain. I have a mekanika cnc table with brackets mounted at certain points for different products. We mount a raw material to this bracket to be sure it's position is always the same.
Now every time i switch to another product(other bracket/place on the table) i have set the x/y zero point. Is there a way to just save this predefined zero points with a name and recall them in the software when is like to set the x/y zero for this product?

Similar Threads:

• Table tilted to save space
• Save actual position
• Tool Table Save / Print ?
• Mach3 tool table save / print ?

[joeavaerage]

Hi,
in Gcode you have different sets of work coordinates. The most common and first on the list is G54, but there are others, G55,G56,G57,G58,G59, G59.1, .......G59.99.
You could store your work coordinates in any one of them. Then when you run the program just call up the previously saved work coords.

Craig

[servtech]

Hi,

Is there a simple way to save a table x/y position in planet cnc?
Let me explain. I have a mekanika cnc table with brackets mounted at certain points for different products. We mount a raw material to this bracket to be sure it's position is always the same.
Now every time i switch to another product(other bracket/place on the table) i have set the x/y zero point. Is there a way to just save this predefined zero points with a name and recall them in the software when is like to set the x/y zero for this product?

Save the program and data after each setup with a program number you recognise for each set up.

[Joostdmx]

Thank you Craig.
As i'm pretty new to planet-cnc, can you tell me how to store a current position to one of this gcodes?
I believe that when i enter just G55 in the gcode window the machine moves to the G55 position so how to store them and where is it stored? Lets say when i reload a full profile with all setup and gui settings in planet-cnc does this gcode get overritten?

Thanks in advance for your time.

[Joostdmx]

Hi
Do you mean by saving and reload a full profile in planet-cnc?
I know about this but the annoying part about that is when i make a small change, for example in the gui, i have to do this again for every profile i saved in the past....

Regards.

[maki]

Hi,
If you didn' solve this problem, here is my example:
- go to settings
- scripts/Koordinate systems/( chose your sys regarding code:G 54, G55 etc)
- pres edit button
- put code into new window:
- f.e. for G55 ( in my case):

G55
G10 L2 P#<_coordsys> X1 Y91
M73 ;store state, auto restore
G17 G90 G91.1 G90.2 G08 G15 G94
M50P0 ;disable speed override
M55P0 ;disable trans
M56P0 ;disable warp
M57P0 ;disable swap
M10P1 ;motor enable
M11P1 ;limits/probe enable
(msg,Move Spindle to work position?)
G53 G00 Z#<_tooloff_safeheight>
G01 F4000
G01 X0 Y0

- save
- exit

in the line G10... end is position of coordinate sys which you can input.
I have also made a 3 buttons on right side to manualy change coo system, named "BtnRight.txt" with text:

cmd: "Machine.Coordinate_System.Select.1" "" image="Icons/IMG_RGT_Coordinate-1.png" imagechange="False" stroke=1 color=#0ffca0 tooltip="Koordinat sys 0"
---
cmd: "Machine.Coordinate_System.Select.2" "" image="Icons/IMG_RGT_Coordinate-2.png" imagechange="False" stroke=1 color=#0ffca0 tooltip="Koordinat sys vacuum"
---
cmd: "Machine.Coordinate_System.Select.3" "" image="Icons/IMG_RGT_Coordinate-3.png" imagechange="False" stroke=1 color=#0ffca0 tooltip="Koordinat sys Kalup"

hope it helps

ps, I am generating cam files with F360 and there is possibility to add coo system when exportin G-code
if you need icons I can post it,

[joeavaerage]

Hi,
I use Mach4 and am not familiar with PlanetCNC procedures. However G54, G55 etc are part of Gcode , they are not specific to any one software solution.

In Mach if I want to populate a particular Work Coordinate System, say G58:
Preparatory: Ensure your machine is Referenced (Homed)
1) Engage G58 by MDI'ing G58
2) Jog to the required work zero
3) Zero each axis required.

Now G58 is populated with the machine coordinates of the work zero of the WCS G58. I don't know how, or when, or even if, PlanetCNC save Work Coordinate Systems, but Mach saves them at shut down.
Thus if you wanted to be sure that the G58 was saved I would shut Mach down and then restart.

To use G58:
1) Start, and Reference (Home) your machine
2) Load your code ensuring that it has a G58 block at the top of the code
3) Run your code.

Note all this really only uses the properties of Gcode. If you wish to automate it then you'd have to start writnig code and that code is specific to each software solution and therefore
code that I might write for Mach would be distinctly different to what you might write for PlanetCNC.

Craig

[ScorpionTDL]

I believe that when i enter just G55 in the gcode window the machine moves to the G55 position so how to store them and where is it stored? Lets say when i reload a full profile with all setup and gui settings in planet-cnc does this gcode get overritten?

entering just G55 will simply load the G55 Coordinate System offset -> restoring the XYZ Zero position that you saved to G55 in a previous step.
The offset coordinates themselves get store in the file CoordinateSystem.txt in you PlanetCNC Profile Directory.
If you want to restore them from a backup you need to shutdown planetcnc replace the file and start planetcnc again.