[jdebott1]

I'm learning and writing G-code for a Shaker Candlestand centerpost, and I need to cut a small radius - see attached.

I'm running Mach3 in mm, and have converted all the inch measurements over. So far, I've completed the rough rounding of the stock and cut the rough taper. Now I'm squaring up the "bulb" portion of the centerpost, but need help writing the G-code for the small radius (3/32 in - 2.3813 mm) on the top of the bulb portion.

I've attached the pics, and if you can give me a hand, I would appreciate it. I've studied the I,J techniques on the web, but I'm still confused a bit on how to do this radius since it begins after the 3/4" straight bit is raised 23.01875 mm from centerline.

Thanks in advance.

Joe D.

[fordav11]

Calculating the radius depends on if you are using G41/G42 tool nose radius compensation or not.

Let's say the OD is 50mm and the radius is 1mm and it starts on the face of the part at Z0.
If you are using G41/G42 then the code is simple....

G0 X48.0 Z2.0 (X start point is OD minus 2 times radius)
G1 Z0
G3 X50.0 Z-1.0 R1.0 (end Z point is the radius amount)

If you are not using G41/G42 you must calculate the tool nose radius compensation yourself (or use CAM software).

Assuming we are using an insert with a 1.2mm radius, for the above example the code will be....

G0 X45.6 Z2.0 (X start point is OD minus 2 times radius and also minus 2 times tool nose radius. i.e. 50-4.4)
G1 Z0
G3 X50.0 Z-2.2 R2.2 (end Z point and R amount is the radius you want plus the tool nose radius)

For internal rads the radius you are cutting (the R) will be the radius you want minus the tool nose radius
If you think about it, with a 0.8R insert if you don't cut any radius, the radius on the part will be 0.8. So you only need to cut the extra amount greater than the tool nose radius.

You should read up on basic programming. The book 'CNC Programming Handbook 3rd Edition' by Peter Smid is a good start point.

[jdebott1]

fordav11,

Thank you for your reply. I did continue to research and learn about cutting these arcs, and I have finally figured out the I,J,K etc and how they work. But, I'm still confused about the radius compensation, and your post helps me quite a bit.

I've been using the web as my main resource, but since my ShopNotes machine is an XZA setup, I can't find much Gcode that directly correlates with my XZA woodworking lathe. So, it's a slow process of trying to read and understand the regular CNC lathe setups and trying to rotate everything to what I am trying to do with my XZA.

I've read excerpts of Peter Smid's 'CNC Programming Handbook' online, and I'll go ahead and purchase it.

By the way, I did work out this small arc that I'm trying to cut after much trial and error on my XZA. I'm now modifying my machine to include a TouchOff, and loading my various woodrouter tools into Mach3. I'll research the G41/G42 code you mentioned and begin trial and error on my XZA. I find it much easier to watch the reaction of the machine than to try and contemplate every Gcode action in my head. Between tweaking my XZA, learning CAD/CAM, MACH3 capabilities, and 3D modeling using GMAX and the CNC Toolkit, my head is spinning round and round.

But, I'll get there with help from nice people like yourself on CNC Zone.

Thanks once again for your help.

JD

[fordav11]

I should also point out that the above radius calculation is valid only for simple 90 degree rads.
if you need to calculate a line to arc or arc to line tangent it gets a lot more complicated.
first you need to use trigonometry to calculate the start/end point then you need to do several calcs using sin, cos & tan to calculate the tool nose radius compensation.
you can read about the method here....
Tool Nose Radius Compensation Lathe Cam

like I said use CAM software to write the program it's a lot easier

[jdebott1]

fordav11,

Hey, a great link!

Thanks again for all your help. I'm setting up my tool setter touch probe now, and trying to read all the new CNC material. There sure is a lot to learn and apply to my unusual XZA lathe.

JD