CAD CAM EDM DRO - Yahoo Group Archive

Re: CNC / DNC

Posted by Jon Elson
on 2000-05-08 16:19:08 UTC
Andrew Werby wrote:

> Re: PROJECTS STILL ON THE BURNER?
>
> It now appears I can get my Beast (the 1984 Leadwell-Ramco) of a
> milling
> machine to accept drip-feed input through its RS-232 port. I tracked
> down
> the people who made the old Centurion IV control (they are called
> Milltronics now, and are located in the Minneapolis area) , called the
>
> number (952-442-1410) and talked to "the old guy in the back". He
> assured
> me that if I could be happy with a 1200 baud rate, could come up with
> some
> kind of "BTR" (Behind The Reader?) box and appropriate shielded
> cables, and
> found a control program that could output my G-code as step and
> direction
> through the serial port of my computer, using Microsoft's built-in
> Hyperterminal or some other null modem connection, then I'd be in biz-
> able
> to feed it unlimited-size files in DNC mode.

This is a muddle. leave out the "output my G-code as step and direction

through the serial port" part, and it makes a lot more sense. There
will
be no step and direction signals anywhere. What you want is a CAD/CAM
program that generates RS-274D (also known as G-Code). This output
generally goes to a file. A number of the CAD/CAM packages have
machine interfaces that can either output step and direction to
stepper motor drivers, or send the G-code through the serial port
(or, in some cases, the parallel port). A 'BTR' (yes, behind the
reader) usually attaches to the parallel port, as it is closest to
the paper tape reader interface.

A CAD/CAM package (or other machine control) will work a lot better
than an off-the-shelf comm program. Especially, in some cases, the
CNC requires the tape to be read backwards (to back up a few program
steps when a tool breaks, for instance).

>
> This sounds distinctly doable (much more so than the Brain
> Transplant), but
> I've got some questions for the experts here:
>
> What control program should I use to communicate with this old DC
> servo-equipped mill? Is this a good excuse to try CNC Pro, or would
> something else be better? Is the DOS port of EMC really ready and for
> sale
> someplace? I think this would go fast enough on my P223, in DOS mode-
> wouldn't the low baud rate be the limiting factor? How many inches per
> min.
> should I expect, in contouring mode?

EMC knows nothing about serial ports, and expects to be directly
controlling the
machine's servo or stepper motors.

>
> Do I really need some special BTR box, or can I go direct from the
> 9-pin
> serial port of my computer? Does this machine need its code fed in
> some
> special way, which the BTR translates from standard
> step-and-direction?

Again, there is NO step and direction, anywhere. Lots of low-end
CAD/CAM
program run step and direction to stepper motors. You don't have these.

Do you have a paper tape reader? Don't be confused by the 25-pin D
plug,
that is not RS-232, it is RS-2xx, a parallel standard for paper tape
readers.
I don't remember the exact numbers, there. But, you may have 2 possible

paths. I didn't have an RS-232 interface on mine, so I made a BTR. I
could
also load the CNC executive from the PC, which was a nice improvement.
But, the RS-232, if it works, will be best for simplicity. Your only
real concern
is to make sure the 'wait' signal is consistant, telling the PC to not
send any
more data until the CNC is ready.


> If
> I do need one, which is the most cost-effective (for an
> non-electronician)?
> What about the "software handshaking" it uses: x-on x-off? How does
> that
> work?

X-on and X-off are two characters in the ASCII code that are often used
for
controlling data flow on RS-232 connections. They have nothing to do
with a
BTR, which uses an electrical signal to control flow. Does your CNC
control
use X-on and X-off? Or, does it use something else, like the clear to
send
signal wire?

> Is this just a series of characters I need to insert at the beginning
> of each program, (and if so, how do I find out what they are?)

No, the CNC would send these characters, if it uses them, to the PC,
which would
stop sending when it receives an X-off, and resume when it sees an X-on.

X-off is CTRL/S, or hex char code 13, decimal code 19. X-on is CTRL/Q,
hex code 11, decimal code 17.

Depending on how your CNC accepts programs from the serial interface,
this may limit what you can do. For instance, a program that returns to
the
beginning and runs again will not work automatically with a comm program

sending from the PC, as it has no way to know the CNC wants to receive
the program again from the beginning. And, if you instruct the CNC to
back up, the comm program won't know how to do this. Each CNC has
it's own little language to express these operations, and a program
specifically
for DNC will know how to handle them. This is really what you are
wanting,
DNC (Distributed Numeric Control), where a central server handles
sending programs to the CNC controls. You can run these completely
from the CNC machine, including writing a program at the CNC control
and uploading it for storage on the PC. To run a part program, you call

it up from the CNC control by name, and the CNC sends a message to
the PC asking for the program by name, and the PC begins to send the
program to the CNC.

Jon

Discussion Thread

Jon Elson 2000-05-08 16:19:08 UTC Re: CNC / DNC Andrew Werby 2000-05-09 10:08:49 UTC Re: CNC / DNC