top of page

Controlling when the machine stops reading a program

All CNC machines made today allow you to transfer program to and from a distributive numerical control (DNC) system. Indeed, you probably transfer programs on a regular basis. An important consideration when reading programs – that is, loading them into the machine – is when the machine will stop reading from the file being sent from the DNC system. With Fanuc controls, one of two settings is possible in this regard. A parameter controls which of the two methods will be used.

First, it is possible that the machine will stop reading as soon as an M02, an M30, or M99 word is seen. These words, of course, are all program ending words. And it may seem logical that the control will stop reading as soon as it sees the first end-of-program word. In my experience, most machine tool builders make this the default setting for the parameter.

Second, it is possible that the control will not stop reading until the end-of-file delimiter is read. For Fanuc controls, the end-of-file delimiter is a percent sign (%). Again, in my experience, this is not how most machines are set.

If you are only loading one program at a time, it really doesn’t matter how this parameter is set. Even if the parameter is set to stop reading when a percent sign is read – and even if there is no percent sign in the program, the control will still read programs (though the machine may not automatically stop reading – you may have to press the reset key).

But if you want to load more than one program at a time – as may be the case when loading a main program and several sub-programs (see the G Code Primer article earlier in this newsletter), you’ll need the parameter set to stop reading when the percent sign is read. If, of course, the parameter is set so that the machine stops reading at M30, M02, or M99, only the first program will be loaded.

To find this parameter, look for the category “CRT/MDI EDIT” in the Fanuc parameter table. For a 16 series control, it happens to be bit seven of parameter number 3201, and has the label NPE (labels tend to be pretty consistent from one Fanuc model to the next). If this parameter is set to a 0, the machine will stop reading at M02, M30, or M99. If set to a 1, the machine will read until a percent sign is seen.

462 views0 comments

Recent Posts

See All

Tapping on a turning center (without canned cycles)

Unless your Fanuc controlled turning center came with live tooling, it’s likely that you don’t have canned cycles (G80-G89) like those you find on machining centers. You might have G74 and G75, the mu

Can you speed up your tool change time?

Machining centers, of course, have automatic tool changing devices to automate the tool changing process. Current models boast very fast tool changing times and you may be quite satisfied with tool ch


bottom of page