# G2 Circular interpolation clockwise direction.

G2- Circular interpolation clockwise direction.

G02- When viewing the gang tools, X1 and Z1, G2 is clockwise. G2X.5W.01R.01

You can also use I J K giving the center of the arc from the position

you start at before the G2. I=X J=Y K=Z G2X.5W.01K.01I0

I,J,K is used when more than a 90 deg arc is needed, usually milling

or turning a ball type part.

G1X.4Z0F.002 or G1X.4Z0F.002

G2X.5W.05R.05 G2X.5Z.05K.05(center of rad is .05 over in Z)

G1Z__ G1Z__

Circle Example…

When milling with or without cutter comp(G41/G42), the feed rate

given is not true. To get a proper feed rate you have to calculate

using the radius desired and the tool radius. Cutting outside

corners are different then inside pockets. Use this formula…

Outside cutting:

DesiredFeed=10 IPM CutRadius=.25 ToolRadius=.125

Feed=DesiredFeed * ((CutRadius+ToolRadius)/CutRadius)

Feed= 10 * ( .375 / .25)

Feed=10 * 1.5

Feed=15

G19

G41G1Z.5Y0 F10.

G2Z.5Y0K.25 F15. (CUT A CIRCLE F15.=F10. at cutting point)

G1Y-.1 F10.

G40

G18

Inside pocket cutting:

DesiredFeed=10 IPM CutRadius=.25 ToolRadius=.125

Feed=DesiredFeed * ((CutRadius-ToolRadius)/CutRadius)

Feed= 10 * ( .125 / .25)

Feed=10 * .5

Feed=5

G19

G42G1Z.5Y0 F10.

X??

G2Z.5Y0K.25 F5. (CUT A CIRCLE F5.=F10. at cutting point)

G1X?? F10.

G40

G18

Also option Helical Interpolation: Same as Circular interpolation

but while 2 axis are circular interpolating, another axis

moves linear. This is mainly used for thread milling, having

to arc X-Y around the thread in circles and move Z down the part.

(center of drilled hole is X.3 Y0 and desired to thread mill 4-40)

G17 G98 G2 X.425 Y0 Z.025 I-.062 J0 P6 F3.

X = X position to go to circular

Y = Y position to go to circular

Z = Z position to linear or if using P then set Z to one pitch.

I = Center of hole from X in radial value.

J = Center of hole from Y in radial value.

P = Number of pitches or threads. Whatever Z is times P

F = Feed rate to cut.