Questions about Fixed Cycle

CNC mill exercise 4C: this is a sample question to illustrate the use of G81 and G83 commands. It is purposely made to change tool to demonstrate the two commands. If you do not need to change tool, it is not necessary to go home (G28).

Using G98 is never wrong. In fact, by default, it is always G98. It goes to the initial plane, making it safe, but wasting time. If you use G99, the danger is there.

You typed polit hole, I think you misspelled the word. It should be pilot hole. It is a hole that is used to guide subsequent drilling. In your first year, you may have leant centre drill. A centre drill acts the same as a pilot hole.

Both G81 and G83 are used to drill through holes, the difference is that if you r drilling a deep hole, you use G83, it may be blind or through hole.

Mostly, holes are drilled using twist drills. In our course, if it is not specified, all holes are drilled using twist drill, tip angle 118 degrees.

Countersink hole can be drilled before or after. However, by drilling countersink hole first, one can use it to serve as a pilot hole, thus saving the effort of machining a pilot hole to guide the subsequent operations.

It is not wrong, if you forget to turn off the coolant and the spindle at the end of the program because G2 or G30 command will turn these off at the end of the program. However, some tools feed the coolant through the tool itself, especially drills. If you forget to turn off the coolant at the end of the machining operation, the tool will carry the coolant when it goes home. (G28) So, it is advisable to turn the coolant off immediately after all the machining operations are done.

G81 is modal, you do not need to repeat it if it is not changed. Same for G98 or G99. So both ways of writing will not be considered wrong. Only that it is not necessary to repeat what is being modal.

Coordinate System

In this first lesson, we talk about Coordinate System. Every workpiece that we machine must have a workpiece coordinate system (WPC) and is defined using G54. There are 3 axes on every coordinate system, one is X axis, running left-right along the machine, one is Y axis, running towards-away from the operator, one is Z axis, running up and down vertically. Once we have this coordinate system, any point or line can be fully described using their corresponding X, Y and Z values. If the points are always defined with reference to the workpiece zero point, it is called absolute position programming (G90). If the points are defined with reference to the current position, it is called incremental position programming (G91).



For every points in the diagram above, write down their respective X and Y values using G90 method, followed by using G91 method.

To machine the workpiece based on the coordinate system, we need to instruct the machine how to cut, from where to where. These instructions are called progamming codes. Every program comprises of blocks, words and addresses.

To instruct the machine simply to move from one point to another, we use the command G0. When we move in air, we can move very fast, making use of the maximum feed rate as provided by the machine builder. To instruct the machine to cut into the workpiece (removing metals along the way), we use the command G1. In this case, however, we need to tell the machine how fast it can move. This is to be defined using the F word. This value depends on what material we are cutting and what kind of tool we are using.

We also need to define the spindle rotation using the S word.

An example program for Mazak machine is as follows:

G0 G90 G40 G94 G21 G17
T1 M6
G90 G54 S597 M3
G0 Z100.0
G0 X-30.0 Y-30.0
G0 Z10.0
G1 Z-20.0 F119
G1 X0.0 Y-30.0
Y110.0
X57.0
Y147.0
X155.0
Y65.0
X42.42 Y0.
X-30.0
Y-30.0
G0 Z50.0
M2

Based on the program given above, can you draw the shape of the workpiece on a piece of paper as an additional exercise?