G2 Circular interpolation clockwise direction.

  1. Home
  2. Knowledge Base
  3. Programming
  4. G Codes
  5. G2 Circular interpolation clockwise direction.
  1. Home
  2. Knowledge Base
  3. Programming
  4. G2 Circular interpolation clockwise direction.
  1. Home
  2. Knowledge Base
  3. TCM S Machine
  4. 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.

Was this article helpful?

Related Articles