G Code with a Mill

[Rion Atkinson]

Originally Posted by sanddrag

The I and J coordinates are the incremental distances from the starting point to the center of the arc, not the coordinates of the center itself. The coordinates of the center itself never actually appear in the code. So if you are starting at 1,5 the center (at 5,5) is located at an incremental/additional 4 in the X (I), and 0 in the Y (J) directions (since you are sitting directly to the left of your intended center).

Also, not sure about yours, but many machines are very particular about leaving decimal points off of a number. For example, on a HAAS machine, "F4" does not mean the same thing as "F4." Oh, and that's the the other thing. You are missing feed rates all around. The units of feed rates are in inches per minute. To start out, I'd keep the feeds under 10 IPM.

Finally, in your first line (the G90 absolute line) I would add G0 X0 Y0 Z1 to make it do what you say in the comment.

Is there a way to change that in the settings of the program? It know the program (And machine itself) I use in my CIM class does not work via increments. So to me his code was just fine. Had he plugged it into the program in my class it would have worked.

Do you have any idea as to what would cause this?

Also. The feed rates depend entirely on what you are cutting. I cut butter board around F15 and plunge at F5 just to be safe. I could probably cut faster. But as a side note. Just as with driving you slow down for turns. Slow your feed rate down when you are cutting arcs.

-Rion

[sanddrag]

Originally Posted by Formerly Famous

Is there a way to change that in the settings of the program? It know the program (And machine itself) I use in my CIM class does not work via increments. So to me his code was just fine. Had he plugged it into the program in my class it would have worked.

Do you have any idea as to what would cause this?

No idea. The standard way G-code is interpreted is how I wrote above. Some manufacturers of machine controllers may choose to differ.

Also, it should be noted that an "R" word in the G02 line is not capable of producing a 360 degree arc. For a full circle, I and J coordinates must be used.

[Cory]

Originally Posted by Formerly Famous

Is there a way to change that in the settings of the program? It know the program (And machine itself) I use in my CIM class does not work via increments. So to me his code was just fine. Had he plugged it into the program in my class it would have worked.

Do you have any idea as to what would cause this?

Also. The feed rates depend entirely on what you are cutting. I cut butter board around F15 and plunge at F5 just to be safe. I could probably cut faster. But as a side note. Just as with driving you slow down for turns. Slow your feed rate down when you are cutting arcs.

-Rion

To clarify, here is an excerpt from the Haas user manual. Note that this is not Haas specific-any Fanuc based controller will follow these same rules. I am certain that his code would not run correctly on your program, as I and J are always incremental distances to the arc's center.

Using I, J, K addresses
I, J and K address are used to locate the arc center in relation to the start point. In other words, the I, J, K
addresses are the distances from the starting point to the center of the circle. Only the I, J or K specific to the
selected plane are allowed (G17 uses IJ, G18 uses IK and G19 uses JK). The X, Y, and Z commands specify
the end point of the arc. If the X, Y, or Z location for the selected plane is not specified, the endpoint of the arc
is the same as the starting point for that axis.
To cut a full circle the I, J, K addresses must be used; using an R address will not work. To cut a full circle, do
not specify an ending point (X, Y and Z); program I, J or K to define the center of the circle. For example: G02
I3.0 J4.0 (Assumes G17; XY plane)

The Haas user manual is a great resource for manual programming. Even though it's put out by Haas, it gives specific examples and sample programs. Like I said earlier, any Fanuc based control will use the same formatting (or very, very similar) as the Haas for all basic g-codes (G00/G01/G02/G03, G43, G41/G42). It's particularly useful for examples involving cutter compensation.

It can be found here: http://www.haascnc.com/pdf/96-8000.pdf

[Rion Atkinson]

Originally Posted by Cory

To clarify, here is an excerpt from the Haas user manual. Note that this is not Haas specific-any Fanuc based controller will follow these same rules. I am certain that his code would not run correctly on your program, as I and J are always incremental distances to the arc's center.

You said that his program would most likely not work on mine. But the way I have been writing programs says that it would.

Here is a program I have written the does indeed work.

;Rion Atkinson
;12-1-09
;Ornament Project
G90 M03 S250 ; Turn on spindle
G00 X0 Y0 Z1 ; Move to starting point
G00 X1.0 Y0.3 ; Move rapid above point A
G01 Z-0.125 F5 ; Plunge to point A
G01 X0.9 Y0.5 F20 ; Cut to point B
G01 X1.9 Y1.4 ; Cut to point C
G02 X2.3 Y0.6 I2.1 J1.0 ; Cut Clockwise to point D
G01 X2.2 Y0.8 ; Cut to point E
G03 X2.0 Y1.2 I2.1 J1.0 ; Cut Counter-Clockwise to point F
G01 X1.0 Y0.3 ; Cut to point A
G01 Z1 ; Move up out of material
G00 X2.0 Y0.3 ; Move rapid above point G
G01 Z-0.125 F5 ; Plunge to point G
G01 X2.1 Y0.5 F20 ; Cut to point H
G01 X1.1 Y1.4 ; Cut to Point I
G03 X0.7 Y0.6 I0.9 J1.0 ; Cut CC to point J
G01 X0.8 Y0.8 ; Cut to point G
G01 Z1 ; Raise up out of material
G00 X1.5 Y1.2 ; Move rapid above point M
G01 Z-0.125 F5 ; Plunge into material
G02 X1.5 Y1.2 I1.5 J1.55 ; Cut Clockwise to point M
G01 Z1 ; Raise up out of material
G00 X2.3 Y1.4 ; Move rapid above point N
G01 Z-0.125 F5 ; Plunge into material
G03 X2.3 Y1.4 I2.5 J1.6 F20 ; Cut CC to point N
G01 Z1 ; Raise up out of material
G00 X0.8 Y1.5 ; Move Above point O
G01 Z-0.125 F5 ; Plunge to point O
G02 X0.8 Y1.5 I0.6 J1.6 ; Cut Clockwise to point O
G01 Z1 ; Raise out of material
G00 X2 Y5 ; Move rapid to off loading point

(Sorry for no line numbers. I had to write this out of a piece of paper so I left them out.

It cut this out of butter board.


http://picasaweb.google.com/lh/photo...eat=directlink

[nighterfighter]

I got bored, so I decided to write this up, hopefully once our mill gets working, I can try it on a wax block.
http://img707.imageshack.us/img707/3061/diamonds.jpg

You can't see it in the picture, but the cuts are different depths...The inner-most circle is the highest, and then each one outside it descends by .25".

I have a quick question about it, will the cuts be too close, and overlap each other?

[Rion Atkinson]

Originally Posted by nighterfighter

I got bored, so I decided to write this up, hopefully once our mill gets working, I can try it on a wax block.
http://img707.imageshack.us/img707/3061/diamonds.jpg

You can't see it in the picture, but the cuts are different depths...The inner-most circle is the highest, and then each one outside it descends by .25".

I have a quick question about it, will the cuts be too close, and overlap each other?

That depends. What is the width of the bit that you plan to use to cut this?

[nighterfighter]

I'm not sure what size we have. I used the smallest one the software had, which is 0.1000"

[Rion Atkinson]

Originally Posted by nighterfighter

I'm not sure what size we have. I used the smallest one the software had, which is 0.1000"

Ok. Well. If that is the width of the bit you can use then the picture shows exactly how it will turn out.

[DonRotolo]

If the lines are more than 0.100 apart, you'll end up with grooves and not a surface.

One might use a 0.250 bit, separate the lines by .250 (maybe .249) and drop down .250.

Just remember that you need to consider what the bit can cut: At that outermost line, you've dropped down by an inch, right? Can your bit cut a whole inch at a time? If not, how might you address that issue?

This is one reason it is often better to learn how to use a manual mill before getting into a CNC mill. Understanding the milling process is critical.

[Ken Ginger]

Look at the following site. http://www.machsupport.com/

Their wizards are very helpful for standard routines. They may offer a break to FIRST teams.
This is the control package team 1189 uses. Our CAD program, Key Creator includes a built in NC function that creates cutter paths and posts them to a wide choice of post processors.

[VEI Dude]

This (free) software may be helpful. It doesn't have a lot of features, but is very simple to use, so you can try it with different-sized endmills... http://www.cncsimulator.com/

Cheers,
-Neil.