On the engineering drawing or 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 engineering drawing or 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 is 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 engineering drawing or 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. At the initial startup 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 are determined with respect to the stationary reference point of Machine Zero.
In order to better understand this concept, this situation can be illustrated with a rectangular plate in which all coordinates are described at their four corners (P1, P2, P3, P4) (Figure 1-21).
P1 = X–15.0, Y–10.0
P2 = X–15.0, Y–12.0
P3 = X–20.0, Y–12.0
P4 = X–20.0, Y–10.0
Figure 1-21 Machine Zero to Workpiece Zero
Determine the coordinates of these points. The rectangle has been placed in such a manner that each side is parallel to one axis of the coordinate system. If the distance from Machine Zero is measured to any point on the workpiece, the coordinates of the remaining points can be determined from the dimensions given on the drawing.
All programmed point coordinates (whose values are determined with respect to Machine Zero) must be calculated with respect to Machine Zero every time, which is time consuming. It may also cause errors due to the fact that all the given dimensions determining the points do not always refer to those on the drawing. As previously mentioned, in order to determine the coordinates for the four corners of the rectangular part illustrated, it is necessary to find the distance between Machine Zero and a specific point of reference on the part. Then, all the remaining dimensional data to be used are taken from the engineering drawing or blueprint.
For all CNC machines, we follow certain principles to define the method of selecting Workpiece Zero from within the part program. At the beginning of the program, we input the value of the distance between Machine Zero and the selected Workpiece Zero by employing function G92 or G54 through G59 for machining centers and function G50 or G54 for turning centers. These measured values are input either directly into the program, as in the case of G92 for mills and G50 for lathes, or in offset registers in the control for G54 through 59. Let us review the same situation as above and note the changes of the point coordinates when applying Workpiece Zero (Figure 1-22).
G92 X15.0 Y10.0 or G54 X–15.0 Y–10.0
P1 = X0, Y0
P2 = X0, Y–2.0
P3 = X–5.0, Y–2.0
P4 = X–5.0, Y0
Figure 1-22 Workpiece Zero Point
The values X15.0 and Y10.0 for G92 or X–15.0 Y–10.0 for G54 through 59 are valid until they are recalled by the same function, but with different coordinates for X and Y. When programming machining centers, we place function G92 or G54 through 59 only at the beginning of the program, whereas the values assigned to function G50 for turning centers will need to be added to the program with respect to each tools position. Once this activation is read by the control, all coordinates will be measured from the new Workpiece Zero, allowing the use of part dimensions for programmed moves.
With turning centers, Workpiece Zero in the direction of the Z-axis is most often on the face surface of the workpiece, and the centerline axis of the spindle is Workpiece Zero in the direction of the X-axis (Figure 1-23).
On machining centers, Workpiece Zero is frequently located on the corner of the workpiece or in alignment with the datum features of the workpiece.
The application of Workpiece Zero is quite advantageous to the programmer because the input values of X, Y, and Z in the program can be taken directly from the drawing. If the program is used another time, the values of coordinates X and Y (assigned to functions G50 and G92 or G54 through G59) will have to be inserted again, prior to automatic operation.
Absolute and Incremental Coordinate Systems
When programming in an absolute coordinate system, the positions of all the coordinates are based upon a fixed point or origin of the coordinate system. The tool path from point P1 to P10, for example, is illustrated in Figure 1-24.
Figure 1-23 Workpiece Zero for Turning Centers Courtesy Kennametal
Figure 1-24 Absolute and Incremental Coordinate System Points
| X | Y | |
|
P
|