Reference Points : Page 3 of 3

The program zero edge should be the fixed jaw - a jaw that does not move. Many programmers incorrectly use a moving jaw as the reference edge. The benefit of programming in the first quadrant (all absolute values are positive) is attractive, but can produce inaccurate machining results, unless the blank material is 100% percent identical for all parts (usually not a normal case). Version 1 setup can be improved significantly by rotating the pan 180° and aligning the part stopper to the opposite side.

In Version 2, results are consistent with the drawing. Part orientation by 180° has introduced another problem - the part is located in the third quadrant! All X and Y values will be negative. Drawing dimensions can be used in the program, but as negative. Just don't forget the minus signs. If the choice is between Version 1 and 2, select Version 2 and make sure all negative signs are programmed correctly. 
Is there another method? In most cases there is. The final Version 3 will offer the best of both worlds. Part program will have all dimensions in the first quadrant, as per drawing. Also, the part reference edge will be against the fixed jaw! What is the solution? Rotate the vise 90° and position the part as shown - next Figure, if possible.

To select a program zero for the Z axis, the common prac-tice is to select the top face of the finished part. That will make the Z axis positive above the face and negative below the face. Another method is to select the bottom face of the part, where it is located in the fixture.

Special fixtures can also be used for a part setup. In order to hold a complex part, a fixture can be custom made. In many applications of special fixtures, the program zero position may be built into the fixture, away from the part. 
Selecting a program zero for round parts or patterns (bolt circles, circular pockets), the most useful program zero is at the center of the circle - Figure below

♦ Program Zero - Lathes

On CNC lathes, program zero selection is simple. There are only two axes to consider - the vertical X axis and the horizontal Z axis. Because of the lathe design, the X axis program zero selection is always the spindle center line.

For the Z axis, three popular methods are used: 

Chuck face          . . . main face of the chuck  
Jaw face             . . . locating face of the jaws  
Part face             . ... front of the finished part 

In setup, a chuck face offers only one benefit - it can be easily touched with the tool edge, using feelers to prevent tool chipping. On a negative side, unless the part rests against chuck face, additional calculations are needed for the coordinate data and drawing dimensions cannot be used easily.
Jaw or fixture face presents more favorable situation. The face can also be touched with the tool and is consistent for all parts. This location may benefit machining irregular shapes, such as castings, forgings and similar parts.
 Many lathe parts require machining at both ends. During the first operation, material stock for the second operation must always be added to every Z value. This is the main reason why CNC programmers keep away from program zero located on jaw or fixture face, except in special cases. 
The most popular method is setting program zero on the front face of the finished part. This is not a perfect selection either but has many other advantages. The only disadvantage is that during setup, there is no finished face. Many operators add the width of the rough face to the setup or cut a small face for the tool to touch. 
What are the benefits of program zero at the front face? One benefit is that many drawing dimensions along Z axis can be transferred directly into the program, normally with a negative value. A lot depends on the dimensioning method but in majority of cases, the CNC programmer benefits. Another benefit, probably the most important, is that a negative Z value of a tool motion indicates the work area, a positive Z value is in the clear area. During program development, it is easy to forget a minus sign for the Z axis cut-ting motions. Such an error, if not caught in time, will position the tool away from part, with the tailstock as a possible obstacle. It is a wrong position, but a better one than hitting the part. Examples in this handbook use program zero at the front finished face, unless otherwise specified. 

TOOL REFERENCE POINT 
The last reference point is related to the tool. In milling and related operations, the reference point of the tool is usually the intersection of the tool center line and the lowest positioned cutting tip (edge). 
In turning and boring, the most common tool reference point is an imaginary tool point of the cutting insert, be-cause most tools have a cutting edge with a built-in radius.
For tools such as drills and other point-to-point tools used in milling or turning, the reference point is always the extreme tip of the tool, as measured along Z axis. Figure shows some common tool tip points.

All three reference point groups are connected. An error in one setting will have an adverse effect on another. The knowledge of reference points is important to understand register commands, offsets and machine geometry.