Understanding G-code ... or not!

[geoff p]

I have just got my (homemade) router to move under computer control.
Now I want to machine some nice 'pockets' to enclose and support the ballraces on the machine, so I found some examples of G-code 'G02' and used them: presto! Damned big circles.

I have tried both 'R' commands and 'Ixx Jxx' commands to make smaller circles but I am totally confused by the codes.

Can anyone explain, in simple English, how they work and what are the parameters?

Thanks in anticipation.

Perhaps some of you could help put together a tutorial about G-codes and their implementation to help the many chip-sweepers coming to this forum?

[Fred Stevens]

The Fadal people have a pretty coherent explanation of programming interpolated arcs, etc. Try the link below:
Fred

http://www.fadal.com/fileadmin/fadal...erpolation.pdf

[Al_The_Man]

Most controls interpret the I,J,K as incremental distance from the cutter position. Also if you are using tool offset G41 G42 make sure it is on the right side.
The advantage with I,J,K method is if the format is wrong it will usually give an error, whereas R will move the cutter regardless.
Al.

[geoff p]

Thanks Fred, the Fadal document looks to be very clear. It certainly covers what I want now (and probably for a fair while.)
Al: I'm afraid I'll have to spend time with the Fadal doc to understand the extra complexity you've just thrown-in.

[Geof]

I assume you want a pocket with a radius larger than the diameter of the cutter you are using so you have to take multiple cuts. Here is one way to do this with minimal complication using a cutter .25" diameter to make a pocket 0.500" deep and 1.500" diameter. Note that I am leaving out all the stuff about selecting tools, speeds, feeds, work zeroes, etc., and just giving the code for the pocket and also assuming your machine interprets G codes in a conventional manner. I am also using both absolute G90 and incremental G91 programming and for G91 I am including the axes that do not move by programming 0.0 incremental movement. These commands can be omitted.

Quick calculations:

1, Pocket radius is 0.750", tool radius 0.125" so for the periphery of the tool to be at 0.75" the center of the tool has to be at a radius of 0.625" so this is your largest radius.

2, Because your cutter radius is 0.125" your smallest radius has to be no larger than this or you will cut a ring and leave a pillar at the center.

3, Because your cutter diameter is 0.25" the biggest increase in radius from one cut to the next has to be less than 0.25". In fact using the full cutter diameter is not good so the increase in radius from one cut to the next in this example is 0.200".

Program:

Move your tool to the position of the pocket center and about 0.05" above the surface of the material:

G91 G01 X0. Y0.1 Z0. (Change to incremental movement and move cutter to 0.1" radius on Y axis; X and Z do not move)

G03 I0.0 J-0.1 Z-0.1 F10. L5 (Incremental is still active; the hole center is 0.1" distance away on the Y axis; i.e. where you started. The cutter is going to follow a counterclockwise path for five full circles and move down 0.10" on the Z axis for each circle so at the end it is at Z-0.45")

G90 G03 I0.0 J-0.1 Z-0.50 L2 (Change back to absolute and clean up the helical ramp and finish this cut to 0.500" deep.)

G00 Z0.05 (Back up to the Z starting position)

G91 G01 X0. Y0.2 Z0. (Back to incremental move cutter to 0.3" radius on Y axis; X and Z do not move. Note you where already at Y0.1 so you moved 0.2 to get a final distance of 0.3)

G03 I0.0 J-0.3 Z-0.1 F10. L5 (Incremental is still active; the hole center is 0.1" distance away on the Y axis; i.e. where you started. The cutter is going to follow a counterclockwise pathe for five full circles and move down 0.10" on the Z axis for each circle so at the end it is at Z-0.45")

G90 G03 I0.0 J-0.3 Z-0.50 L2 (Change back to absolute and clean up the helical ramp and finish this cut to 0.500" deep.)

G00 Z0.05 (Back up to the Z starting position)

I will not continue with the detail to save space.

You now move Y another 0.2 to get a total Y movement of 0.500" and change the J to -0.500.

Then you move Y another 0.125 to get your final Y movement of 0.625", change J to -0.625 and finish the pocket in the final sequence.

Other details can be included in the program: You can use tool compensation so the machine compensates for the tool radius and you program for the actual radius 0.750" rather than 0.625".

You can do things such as moving to your cutting radius by following a circular path that approaches your radius tangentially so there is no witness mark where you machine abruptly changed direction from a straight G01 motion to the circular interpolation.

These refinements can come later when you are comfortable with what you are doing.