Re: getting started with CNC

Jim Wilson wrote: 
Bill Roberto wrote...

Swap 3 and 4. Define your tools before creating G code.


Makes sense.


Also plan your cutting strategy in logical steps. i.e. Rough, rough, finish, finish as opposed to Rough, finish, rough, finish. 


Yes, of course.

So,

1. Design the part using a CAD system.
2. Produce a DWG or DXF file for the part.
3. Define the tooling & assign their ATC locations.
4. Generate a G-code file from the DXF file.
5. Tweak the G-code file if/as needed.
6. Transmit the G-code file to the machine.
7. Load the tooling into the auto changer.
8. Load the workpiece material into the machine.
9. Touch off the tools. [*1]
10. Execute (or possibly drip) the program.
11. Retrieve the finished part.
12. Go back to step 8 until enough parts are done.

[*1] suggested by D Murphy.

Assuming this outline is reasonably accurate, the first "gotchas" I see for me fall in steps 4, 6, 9, and perhaps 10. The rest seem straightforward enough at this point.

It appears from the net (and the archives) that free software is available to generate G-code from DXF. Any specific recommendations? How does the free stuff compare with the expensive commercial offerings? 

They all work. Some better than others. Seat time is the key.


Step 6 "transmit the G-code file to the machine" is the biggest stumper for me at the moment. I am not slowed by RS-232 itself, having worked with computers and serial communications since the mid-70's. However, I have not seen a command set defined for PC-to-(my machine) communications. The information doesn't appear to be covered in the Fanuc 6M Model B manuals I received. Given that the machine is 1984 vintage and has a tape reader, I figure the RS-232 port may have been an option or subsequent add-on, and that a separate reference exists somewhere for the file transfer and control commands recognized by the system. Any guidance on this front?

Once you have your cable correctly configured;(machine side 25 pin) Pins 4 & 5 jumped, pins 6,8, & 20 jumped. pins 2 and 3 go to 2 and 3 on the computer side (9 pin) 7(25 pin) goes to 5(9 pin). Press "read" on the control and it should blink "lsk" while it listens for your computer. Set you communication parameters to 7 data bits, 1 stop bits, and even parity. Your baud rate is probably 4800. Fanuc usually sets it there at the factory.


Step 9 "touching off the tools" raises some questions, also. I confess the phrase is new to me. From the sound, I guess it refers to determining z-axis offsets for the tools loaded into the tool holders. Even if this is right, though, I'd be interested in hearing specific techniques for accomplishing it. My machining experience is limited to manual machines.

You will have at least 2 different offsets. One will be your fixture offset G54-G59. This is the distance from your machines home to the parts X and Y position. The other offsets are designated with a G43 and a corresponding H value. The H value is the distance from the machines home to the part in Z. You will have one fixture offset and as many height offsets as you have tools.


I'm hoping my Step 10 "execute the program" questions will be covered when I get the machine's instruction manual, which was delayed. I would think, though, that with a machine as old as this and with limited memory (32K, IIRC), drip-feeding the code might be necessary for even moderately complex parts. I presume there is readily available software that does this. Any recommendations on this one?

Make sure you dry run your program above your part before trying to cut anything. You can catch big mistakes before they happen. Most software packages have at least communications for uploading and downloading code. Drip feeding is usually an option.


Thanks for the feedback so far, and for anything else you can offer.

Happy New Year!

Jim 
.