Drive commands2.1 Interpolation commandsISO Milling20 Programming Manual, 06/09, 6FC5398-7BP10-1BA0Element Command DescriptionDirection of rotation G02 clockwiseG03 counterclockwiseEnd-point position Two axes from X, Yor ZEnd-point position in a workpiece coordinatesystemTwo axes from X, Yor ZDistance of start point - end point with signDistance between start point -centerTwo axes from I, J orKDistance start point - circle center with signRadius of circular arc R Radius of circular arcFeed F Speed along the circular arcDesignation of the planeWith the commands specified below, a tool traverses along the specified circular arc in theplane X-Y, Z-X or Y-Z, so that the feed specified with "F" is maintained on the circular arc.● in Plane X-Y:G17 G02 (or G03) X... Y... R... (or I... J... ) F... ;● in Plane Z-X:G18 G02 (or G03) Z... X... R... (or K... I... ) F... ;● in the Plane Y-Z:G19 G02 (or G03) Y... Z... R... (or J... K... ) F... ;Before the circle radius programming (with G02, G03), one must first select the desiredinterpolation plane with G17, G18 or G19. Circular interpolation is not allowed for the 4th and5th axes, if these are linear axes.Plane selection is also used to select the plane in which the tool radius compensation(G41/G42) is performed. The Plane X-Y (G17) is automatically set after activating the controlsystem.G17 X-Y planeG18 Z-X planeG19 Y-Z planeThe working planes should be specified, in general.Circles can also be created outside the selected working plane. In this case, the axisaddresses (specification of circle end positions) determine the circular plane.Circular interpolation is possible in the Xβ, Zβ or Yβ plane while selecting an optional 5thlinear axis, which also contains a 5th axis besides the X-Y, Y-Z and Z-X planes (β=U, V orW)● Circular interpolation in the Xβ planeG17 G02 (or G03) X... β... R... (or I... J... ) F... ;● Circular interpolation in the Zβ planeG18 G02 (or G03) Z... β... R... (or K... I... ) F... ;
