G54, G55, G56, ...
Hi,
I often machine identical parts and would like to machine several of them at the same time. I could secure them to the table then probe the datums and copt/translate my toolpaths in the CAM package, post process and run but this is rather time consuming (500K lines of code). What I would like to do is probe the datums of each work piece and enter them into a script that will change the X,Y,X zero values after cutting the first part then run the program again etc. Even adding gcode at the end of the program then pasting a copy of the program below would do.
Any ideas anyone?
Thanks
Similar Threads:
G54, G55, G56, ...
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Thanks, obviously I am quite new to this but did manage to find the G54,G55 etc
So if I set XYZ to zero at fixture datum #1
G54 0 0 0
G55 at distance from datum #1 to datum #2
will this code work?
G21
G90
G91 G28 X0 Y0 Z0 M05
(T1 End Mill D8 )
G90 M6 T0101
(----------------------------------------------------------------- )
M03 S2400
G00 X-4.1200 Y89.0000 F1000
G00 Z1.0000 F400
G01 Z-1.5000
G01 Y0.0000
G01 X-4.0000
etc
G01 Y0.0000
G01 X-4.0000
G01 Y89.0000
G00 Z-5.2500
G00 X-4.1200
G01 Z10.0000 F1000
G55
repeat G code
G91 G28 X0 Y0 Z0 M05
G90
M30
You do not mention what size CNC you have, nor what controller you have (eg Mach3). This info is usually needed.
I have machined up to 20 units at a time, in a 3x6 or 2x10 grid, using the G54/etc codes.
Or you can simply do the maths yourself in your code. Um - if you are using a dum CAM package, that might be more difficult. I write my own programs by hand.
Cheers
Roger
Whoops - I did mean G55 not M55.
I will have a play tomorrow with G55 as if I get it eorking it will be a great help as I will be able to machine 4 parts overnight.
Last edited by luremaker; 08-19-2019 at 06:28 PM.
Be warned: there is a slight problem in Mach3 with G54.
When you load a program which is written using several instances of G54, the on-screen display of the cutter path at Load Time is correct, but the Run-Time display is not. The run-time display SW forgets all about the offsets. This is clearly a display bug in Mach3 as a) the load-time display is correct and b) the actual path machined is correct. One gets used to this ... (I think it was an error by the original author: Art Fenerty.)
So why didn't Artsoft fix this? Two reasons: not enough loud complaints about it, and then they decided to go for Mach4 instead. One day, someone is going to get hold of the source code for Mach3, strip the LPT driver stuff right out (ie rely on the ESS), and fix the bugs. That may take some doing ...
Cheers
Roger
Well had a go today with a small program.
Set G54 to datum of first part and G55 to datum of the second and it ran OK.
BUT I then set G54 and G55 to 0,0,0 loaded a workpiece and set the datum and ran my program and at about line 19,000 the machine decides to go to machine 0,0,0 then back to the workpiece and carried on cutting. There were no lines in the gcode calling for this move so it beats me.
Mach3 has lots of little bugs that only show up on occasion. And different versions may have different bugs.
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Thats why I went to Mach4, too many little unexplained glitches.
1000x750 Workbee CNC - Mach4 - PMDX USB - Windows 10 Pro
If you just cut and pasted the first program then called it G55 then yes it will have a start position at the first part in it, and will go back to the first part, you have to be careful when you cut and paste in programs as this will happen nothing to do with the control it's doing what you are telling it to do
Mactec54
Mactec is right. Doing a cut&paste without checking the guts of the file is going to fail 99.99% of the time.
How many CAM programs can handle anything beyond G0-G3 and simple drilling? Rather few I think.
Cheers
Roger
Here's one that handles a few LinuxCNC "G-Code" Quick Reference . Not heavily promoted and not from Artsoft,so maybe out of place here.Its also free so you can try it for absolutely nothing.
Thanks for all the help folks it is really appreciated.
Am I correct that G54 is the default datum in mach3 and if this is the datum for the first part, would I be correct that if I add a G54 line to my code after the last cut then when load anther program it should start with the correct datum for the first part?
I do modify my code for several reasons and to ensure the correct datum is used I add the following lines at the start of each program after the tool change
G00 X0.0000Y0.0000
(Check X and Y datum, press Cycle Start to continue)
M00
G01 Z10.000 F500
(Z is at +10mm , press Cycle Start to continue)
Also mactec54 why "never use a Z axes move when Doing a X Y move, a Z move should always be on a line before a X Y Axes move for obvious reasons"? Most of my work is 3D surfaces so a lot of the code has x,y,z moves on the same line. If anything I would expect it to be safer to move in X and Y then plunge in Z unless cutting flat bottomed pockets.
3D surfaces have nothing to do with X Y Z rapid moves to the start of a part, or a new position move, the Z axes is always moved first then a X Y move the reason you move the Z first is so you don't crash into your work piece as X and Y will move first then Z axes which In most cases is to late the crash has happened
G54 is the default in all machines controls until you change it in your program
Only your first part would be at G54 X0.0 Y0.0 you next part work offset would be the distance to the start of the next part G55 X----Y0.0 one or both of the axes X and Y will have a different start point than the first part the Z axes does not change unless the work height changes
Mactec54
Well all is going well using G55 and as RCaffin says the run time display sometimes forgets that G55 has been used and displays the cuts s though G54 was used.
I am now machining up to 4 parts all with different Z datums. I load all the parts and probe their X,Y datums (G54,G5 etc) with a 4mm dowel in the collet, the correct tool is loaded and usng a macro Z is probed on all parts and the program run.
In order to save time I would like to ust load the next tool and have Mach3 automatically probe Z on all the parts. I have found out (or led to believe) Mach3 cant call macros so does anyone know of a solution?
I have found out (or led to believe) Mach3 cant call macros
That is totally and utterly FALSE.
In fact, the G73 instruction is actually executed by a called macro.
Probing is always done with a rather large Macro call: there are many versions.
In essence, Mach3 using Crystal Basic, which is someone's implementation of Basic as an linkable library.
If you can do it in Basic, you can do it in Mach3.
Mach4 uses LUA instead - I don't know why Artsoft changed. But basically (sorry!) it's the same thing.
For a start, you want the Mach3 V3 Programmers Reference manual, for Mach3-specific calls. Two flavours: V3 and V3.x
Next, you want the VBScript_Commands.pdf file by Crystal Basic for some deeper info.
Mach_VB_Parameteres.doc is an essential guide to accessing Mach3 variables in Basic.
Cypress Basic.pdf is obviously going to be useful.
All these are to be found on the Artsoft web site somewhere. They do have a lot of doco support for you.
There is a doc called Coordinate Spaces: a Guide, at Coordinate Spaces - a Guide (I wrote it).
You can also search the CNCZone web site for other docos. There is a lot around the web.
If you are coming from a Fanuc world, please note that Mach3 allows you to call g-code subroutines anywhere: I believe they are the same thing as Fanuc's Macros.
For all that some people pooh-pooh Mach3 in favour of Mach4, it is still an extremely powerful tool for running a CNC. It has a few bugs, sadly, but many people make a living from Mach3.
Cheers