Programming of CNC Machines. Ken Evans
coordinate but will give a polar system in the form of an angle for the location of a feature. With some basic trigonometric calculations, this information can be converted to the rectangular coordinate system.
The same polar coordinates system applies regardless of the axis of rotation as is shown once again in Figure 14. When rotation is around the X axis, the rotational axis is designated as A, the Y axis, the rotational axis is designated as B, and the Z axis, the rotational axis is designated as C. These are considered an additional axes and are known as the fourth axis.
All operations of CNC machines are based on three axes: X, Y, and Z.
1. (X0, Y0, Z0)
2. (X0, Y0, Z+)
3. (X0, Y-, Z+)
4. (X0, Y-, Z0)
5. (X-, Y-, Z0)
6. (X-, Y0, Z0)
7. (X-, Y0, Z+)
8. (X-, Y- Z+)
Figure 15
Figure 15 illustrates a box-like object in which one vertex (point 1) is located at the origin of the coordinate system. At the side of the drawing, the coordinate signs are given for each the numbered locations. Note the position of the coordinate system on the following machines.
Figure 16 Axis Designation for a Three Axis Mill
On vertical milling machines the spindle axis is perpendicular to the surface of the worktable.
Figure 17 Axis Designation for a Three Axis Horizontal Mill
On lathes, the spindle axis is also the workpiece axis.
Figure 18 Axis Designation for a Two Axis Turning Center
On horizontal milling machines the spindle axis is parallel to the surface of the worktable.
When using CNC machines, any tool location is controlled within the coordinate system. The accuracy of this positional information is established by specific Zero Points (reference points). The first is Machine Zero, a fixed point established by the manufacturer that is the basis for all coordinate system measurements. On a typical lathe, this is usually the spindle centerline in the X axis and the face of the spindle nose for the Z axis. For a milling machine, this position is often at the furthest end of travel in all three axes in the positive direction. Occasionally, this X axis position is at the center of the table travel.
This Machine Zero Point establishes the coordinate system for operation of the machine and is commonly called Machine Home (Home Position). Upon startup of the machine, all axes need to be moved to this position to establish the coordinate system origin (commonly called Homing the machine or Zero Return). The Machine Zero Point identifies to the machine controller where the origin for each axis is located.
The Operator’s manual supplied with the machine should be consulted to identify where this location is and how to properly Home the machine.
The second zero point can be located anywhere within the machine work envelope and is called Workpiece Zero and is used as the basis for programmed coordinate values used to produce the workpiece. It is established within the part program by a special code and the coordinates are taken from the distance from the Machine Zero point. The code number in the program identifies the location of offset values to the machine control where the exact coordinate distance of the X, Y and Z axes of Workpiece Zero is in relationship to the Machine Zero. All dimensional data on the part will be established by accurately setting the Workpiece Zero. A way of looking at the Workpiece Zero is like another coordinate system within the machine coordinate system, established by the Home Position.
Tool offsets are also considered to be Zero Points as well and are compensated for with Tool Length and Diameter Offsets. The tool setting point for a lathe has two dimensions; the distance on diameter from the tool tip to the centerline of the tool turret, and the distance from the tool turret face to the tool tip. The tool setting point for the mill is the distance from the spindle face to the tool tip, and the distance from the tool tip to the spindle centerline.
Blueprint Relationship to CNC
The standard called ASME Y14.5-1994 establishes a method for communicating part dimensional values, in a uniform way, on the engineering drawing or blueprint. The drawing information will be translated to the coordinate system in order for dimensional values and part features to be manufactured.
On the blueprint, Datum features are identified as Primary (A), Secondary (B) and Tertiary (C). Dimensions for the workpiece are derived from these datum features. On the drawing, the point where these three datum features meet is called the origin or zero point for the part. When possible, this same point should be used for Workpiece Zero. This allows the use of actual blueprint dimensions within the part program and often results in fewer calculations. Most drawings are developed using an absolute dimensioning system based on Datum dimensions derived from the same fixed point (origin or zero point). Occasionally, some features may be dimensioned from the location of another feature. An example of this might be a row of holes exactly one half of an inch apart. This type of dimensioning is called relative or incremental.
Note: A thorough knowledge of blueprint reading is imperative for successful results using manual or CNC equipment.
Machine Zero
Each CNC machine is assigned a fixed point, which is referred to as Machine Zero (or Machine Home). For most machines, Machine Zero is defined as the extreme travel end position of main machine components that are oriented in a given coordinate system. From Machine Zero, we can determine the values of the coordinates that, in turn, determine the position of the points commanded in a CNC program. Electromechanical sensors called micro-switches (limit switches) are located in the extreme end positions of traveling machine components. These sensors send a signal to the controller when they are activated and thus setting the Home position. In the case of milling machines, Machine Zero on the table is set with respect to the X and Y axes. Machine Zero on the spindle is set with respect to the Z axis, whereas Machine Zero of the tool carrier on lathes is set with respect to the X and Z axes. Positioning the traveling components at zero can be performed manually, as well as with the use of the control panel or directly from within the program by employing a Reference Point Return function (G28). At the initial start up of any CNC Machine, it is required that the machine be “Homed” or sent to Machine Zero before proceeding any further. From that point on, all machine components will always automatically return to the same exact position when commanded to do so in the program.
Machine Zero is frequently the position in which tool changes take place. Therefore, if you intend to change the tool before a given operation, then the machine must be positioned at Machine Zero for the Z axis on vertical machines and the Y axis on horizontal machines.
Workpiece Zero
So far, for all main traveling components of CNC machines, we have assigned an oriented axis within the coordinate system. Any movement of machine components must be described by points, which actually determine the traveling path of the tool. Changes in the position tool