[CAMmando]

Good stuff guys ... Just thought I'd pile on a couple of thoughts.

--- Modality---

G2/G3 are modal (in most machines.). Meaning that they stay active until cancled by another modal command in therir "Group". This would include G1, G2 or G3, Canned Cycles like G81 etc. Check the code list in your manual.

So after calling a G2, the next arc move does not require you to call another G2, Just the appropriate X Y Z I or J.

--- Helical Interpolation ---

If your control supports helical interpolation, this is usualy acomplished with a G2 o G3 that contains a Z Value in addition to X Y I & J. In this case all of the other values work the same.

-- Arcs in other planes ---

Most Fanuc type controls spend most of their life in the G17 (XY plane). Your programs prolly have a G17 up near teh beginning, and maybe before and or after a toolchange.

G17 is a modal command that tells the control to generate movement in the X,Y axis. (ie. the arc centerline is paralell to the Z axis). For working in other planes, you can still use the G2 or G3, But you must first tell the control to change planes. G18 and G19 is commanded to use XZ or YZ Arcs (centerline paralel to X or Y axis). For an example of this, toolpath an YZ Arc in Mastercam. Depending on how your post is set up and whether uo comp to the tip or the center of a ball mill you may need to check the filter box. Post the code and check it out. You should see a G18 or G19 then your G2 or G3. Notice the X or Y is replaced with Z.

A point of interest here. If you (or your post) dont command G17 before you change tools, you will probably receive an error message that seems to make no sense. The machine will be telling you it cant Go Home or to tool change position because the coordinate system is all goofed up.

To get really tricky you can use polar coordinates and do pretty cool stuff with G2 and G3 (machine domes etc.) that would be a topic for another day.

Hope that helps.