# Thread: How to put a radius on the outside corner of a square?

1. ## How to put a radius on the outside corner of a square?

I am building a box with a lid. When I cut the inside of the box out I get a nice radius on each corner since the mill is round. I am cutting a lid to fit down in the opening with edges that are flush with the outside of the box. My problem is that I can't figure out what G Code to use so that the corners of the lid that go inside the box are the same radius as the inside corners of the box? I keep getting square corners any time I cut an outside square. I'm guessing the I and J coordinates, but just can't figure out how to get them to do it. Thanks in advance for any help you can provide so that I can get this square peg into the round hole.

Randall

2. You need to program the path for the radius you desire. Program the radius that is the same as the end mill you used for the inside of the part (if you used a .500 end mill, you will program a .250 radius). I use a Haas mill, and it allows me to program a radius using the "R" command only, but you can also do it using I and J (I being the centerpoint of the radius in X axis, J the centerpoint in Y axis). Picture a 4" x 4" square box with .250" radiused corners:

T1 M06
G00 G90 G54 X-.5 Y-.5
S3000 M03
G43 H01 Z.100
G01 Z-.5 F5.0
G01 G41 X0 Y-.100
G01 Y3.75 F10.0
G02 X.25 Y4.0 R.25
G01 X3.75
G02 X4.0 Y3.75 R.25
G01 Y.25
G02 X3.75 Y0 R.25
G01 X.25
G02 X0 Y.25 R.25
G01 X-.5
G00 Z3.0
G00 G40 X0 Y0
M30

This code will cut the square with radiused corners by climb cutting, with left cutter compensation. If your mill does not read radii with R commands only, add the centerpoint of the radius using I and J to the lines with the R commands.

Hope this helps!

3. I think I'm getting a better understanding of how it works. I'm using Turbocnc on a homemade cnc router so I'm thinking the I and J are going to be necessary. I'll have to do some experimenting. Thanks for the tips.

4. If you're using TurboCNC, you'll need to remove the G41 and G40. TurboCNC doesn't yet support Cutter Comp.

• Is there any mill controls that could calculate radius so I would not have to calculate start point?
Many lathes have it.
Program would go something like this:

G01 Y4.0 F10.0 R.25
G01 X4.0 R.25
G01 Y0 R.25
G01 X0 R.25
G01 Y.35
G01 X-.25
G00 Z3.0