91ÊÓƵÍøÕ¾ÎÛ

Ideally, CNC machines should be completely automatic. Once a cycle is activated, the machine should run the entire program without stopping. In this way, and with an acceptable process, the operator is free to perform other tasks while the machine is running. Additionally, the time required to complete the production run will be more consistent and predictable. This is especially important with larger lots.

While completely automatic operation should always be the goal, and you should never be too quick to give up on it, there are situations that require operator intervention during the CNC cycle. Each requires its own special considerations. Here are four suggestions based on how often an intervention is required:

At the operator’s discretion, first instance

This first suggestion is quite popular. Since metalcutting CNC machines can hold several cutting tools, most programmers choose to include an optional stop command (M01) at the end of each tool. The optional stop switch on the operator’s panel then lets the operator easily control whether the machine will stop at the end of each tool.

This is especially helpful while running the first workpiece. The setup person can check what each tool has done prior to moving on to the next tool. It is also required for trial machining, a technique that lets the setup person or operator force each finishing tool — when machining for the first time — to machine surfaces within their tolerance bands and very close to their target values.

At the operator’s discretion, second (or more) instance

Placing an optional stop command at the end of each cutting tool eliminates the ability to (feasibly) use M01 for anything else. If there is a need to provide the operator with the ability to stop the cycle for any other reason, M01 cannot be used. Otherwise, the machine would stop at the end of every tool as well.

Maybe you want to give the operator the ability to check a cutting tool’s insert during a very long roughing operation, and replace it, if necessary. They may not want to do so for every workpiece — only after several workpieces have been run when they begin to suspect excessive tool wear. Again, if an optional stop command is used at the end of each cutting tool, it cannot be used for this purpose.

One way to provide a “second optional stop” involves optional block skip (also called block delete), specified with the slash code (/). Consider this command:

• /N235 M00

If the optional block skip switch is on, the CNC will skip the program stop command. This would be the case when the finishing tool’s insert is fresh. When the operator wants to check the insert, they will turn off the optional block skip switch. Now the CNC will execute the M00 command and stop.

Another way to accomplish a second (or third, or fourth and so on) optional stop application is to use parametric programming commands. An IF statement could perform the required test to see whether the machine should stop. The operator could, for instance, set a variable that tells the IF statement how to behave.

In every cycle

If you have an application that requires operator intervention in every cycle, simply use a program stop (M00) command. Example applications include reducing clamping pressure in the workholding device prior to finishing operations, blowing chips out of the work area after lengthy roughing operations and prior to finishing, and adding tapping compound prior to tapping operations.

My only suggestion here is that you include a message in or after the M00 command that tells the operator what it is that they are expected to do:

• N180 M00 (TURN PART AROUND IN CHUCK)

The message will only be visible if the operator is monitoring the program display screen page. If the machine has Custom Macro, the following command (called a stop-with-message command) can be used that will stop the machine and force the message to be displayed:

• N180 #3000=100 (TURN PART AROUND IN CHUCK)

After a given number of cycles have been run

The last method we offer involves making the machine stop during a cycle only after a given number of cycles have been run. For example, after every fifth workpiece has been machined, you want the operator to check a machined surface right after the cutting tool machines it. Our suggestion requires parametric programming techniques to set up a kind of loop. Here is an example, given using FANUC Custom Macro:

• O0001 (Main program)
• (Ensure that #500 is set to 0 for first workpiece)
• .
• .
• .
• N190 (Finish turning tool)
• (Perform machining operation)
• .
• .
• (Loop for stopping during every sixth part)
• #500=#500+1 (Step loop counter)
• IF [#500 LE 5] GOTO 250
• #500=0 (Reset loop counter)
• #3000=100(CHECK 1.75-IN DIAMETER)
• N250 (Program continues)
• .
• .
• .

What can be done to eliminate the intervention?

As mentioned earlier, stopping programs for operator intervention should only be done after exhausting all automatic alternatives. For examples that stop during every cycle (adding tapping compound, blowing out chips or reducing clamping pressure), and probably many others, there are programmable functions available as machine accessories. Of course, purchasing the related machine accessory will save countless hours of operator intervention during the course of a CNC machine’s life.