What Is Cylindrical Interpolation?
Machine tool builders can provide special interpolation types based upon their customers' specific needs. Some three-axis (X, Z and C) turning centers, for example, are equipped with live tooling.
Founder and President, CNC Concepts Inc.
Machine tool builders can provide special interpolation types based upon their customers' specific needs. Some three-axis (X, Z and C) turning centers, for example, are equipped with live tooling. And if the CNC user will be performing contouring operations parallel to the spindle centerline, polar coordinate interpolation (discussed in a previous CNC Tech Talk column) will allow programmers to "flatten out" the rotary axis. For programming purposes, they can treat the rotary axis as if it is a linear axis. Since not all end users require this ability (even those who do have turning centers with live tooling), polar coordinate interpolation is a field installable option.
Though it is not at all a common machining operation, some machining center users do have a similar need. They must mill around the outside diameter of a round workpiece while incorporating a rotary axis movement (A, B or C) in conjunction with an X- or Y-axis motion. The milling operation commonly occurs with the center of the cutting tool right on the center of the workpiece in one of the axes (X or Y).
Programming this operation can be difficult (especially for any circular movements involving the rotary axis), and as you may have guessed, cylindrical interpolation will dramatically simplify programming. Just like polar coordinate interpolation for turning centers, cylindrical interpolation will allow the programmer to flatten out the rotary axis movements, treating them like linear axis movements.
Figure 1 shows the coordinate system for cylindrical interpolation. For this example, the rotary axis is parallel to the X axis (so it's called the A axis). The horizontal base line represents the A axis. The range for the A axis in this coordinate system is from 0 to 360 degrees. The vertical base line represents the X axis. A tool path is shown that will send the tool all the way around the workpiece in the A axis. This tool path is showing the centerline path for the cutter. The tool will be right on the center of the workpiece in the Y axis (center of the workpiece is program 0 in Y).
Note that when it comes to the circular motions, the angular departures must be appropriate and be based upon the workpiece diameter. The larger the diameter, the larger the angular departures are for circular motions. A coordinate sheet (Figure 2) approximates the rotary axis departure.
Here is a sample program that shows the use of cylindrical interpolation.
00001 (Program number)
N005 G54 G90 5500 M03 (Select coordinate system, absolute mode and start spindle)
N0 10 G00 X3.0 Y0 A0 (Move into position in X, Y and A, point number 1)
N0 15 G43 H0 1 Z3.1 (Rapid to within 0.1 of work surface, part is 6 inches in diameter)
N020 G0 1 22.75 F4.0 (plunge to machining surface)
N025 607.1 A2.75 (Invoke cylindrical interpolation, machining radius is 2.75 inches)
N030 G01 A55.0 F10.0 (Feed to point 2)
N035 G02 X2.5 A90.0 80.5 (Circular move to point 3)
N040 G01 X1.5 (Feed to point 4)
N045 G03 X1.125 A120.0 80.375 (Circular move to point 5)
N050 G01 A165.0 (Feed to point 6)
N055 X3.0 A270.0 (Feed to point 7)
N060 2360.0 (Feed to point 8)
N065 Z3.1 (Retract)
N070 607.1 A0 (Cancel cylindrical interpolation)
N075 G91 G28 X0 Y0 Z0 (Go to 0 return position)
N080 M30 (End of program)