[WarrenW]

What I mean is for Mach 3 compared to other programs - are there different gcode commands for certain things? Or is it standard for all software and drivers? The reason I ask is when you run SheetCam it asks what software you will be using and I just assumed that was for generating the gcode.

I'm working on my own application in VB6 that will take any text and/or image and create the DXF or GCode to use in the driver software like Mach 2/3. It will support many features like the cutting depth, cutting increments, etc. Like SheetCam it will also determine the proper toolpath if your doing cutouts for letters so it does the inside cuts first. Nothing really fancy but I'm having fun writing it.

Warren

[ger21]

The standard codes like G00, G01, G02 and G03 arte pretty standard, as well as quite a few others. But some can be quite different, like canned cycles and M codes. Just about all controllers are a little different, which is why you usually have a post processor for each different control. Some may not support certain codes, others need a different "header" in the file, there can be lots of little differences. But if you use the basic codes like I mentioned, as well as a few others, you can write g-code that will run on almost all machines.

[Al_The_Man]

Also there are some differences between types of machines, Mill, Lathe, EDM, Plasma etc each have some M & G codes that have become standard to their operation.
Al.

[tq9516pjm]

Warren, I am building my first 3axis machine for jewerly making and do a lot of VB programming. If you are running short on time for banging out code, i would be willing to work with you. (if you are developing an app which you wish to sell and do not feel comfortable working with anybody else, i understand.)

[fredhh47]

It is also important to be aware of the unfortunate fact that different controllers interpret the same G-code in different fashions. This is very prevalent in the interpretation of circular commands, as some will interpret the "I" and "J" values as absolute dimensions and some will see them as incremental, some circular commands need the absolute start and end points, some use the absolute start points and the incremental distances to the end points, etc, etc. There are a lot of subtle variations that make it a necessity for you to pretty much have a post processor for every control you have. Even among machines from the same manufacturer, such as Bridgeport, different machines need different information. For instance, an original BOSS 5 will only use three digits after the decimal point in any dimension. Since it only positions in .001 increments, more is just excess characters in a very limited capacity memory. A BOSS 6 will read 4 digits after the decimal point, but rounds to the nearest .0005. In many applications, you can use a BOSS 5 post for a BOSS 6 with minimal loss of accuracy. A BOSS 9, or higher control will read 5 digits after the decimal, but four is more than enough for most situations. Also they can handle text in the program which would cause earlier controls to freeze. So, the LONG answer is there are a lot of variations in G-coding for different machines. You really have to become acquainted with each machine and have a dedicated POST for each one.

[WarrenW]

Thanks, I don't think I'll have too much trouble since all arcs are made up of lines in my software. So all I need to do is move it in lines and I can setup an options area for any code that still may be different for each machine. My app is just for 2D cutting right now.

Thanks!

Warren