practical Edgecam

[crazycnc]

Hello all,
I have been using Edgecam for a bit over a year now, and am getting to like it better the longer I use it. I am mostly self taught although I did take a few days training at the local resellers. I am trying to automate the total programming process more so that there is less room for errors to creep in.
We run a lot of two sided parts on our lathes. (Face the first side, maybe drill and bore a hole, then flip it around and face the back side, or some variation of this). What I typically do is create two CPLs and two nc programs. The first program I number as 101, the second one as 102. Then I'll manually make another program, something like this:

:0100
M98P0101
M5
M00
G00X5.0Z9.0
G50X5.0Z9.06
M98P0102
G00X5.0Z9.06
G50X5.0Z9.0
M5
M30

(Note that I usually require an offset between the two sides, which is what the G50 is doing, offsetting the coordinate system by 60 thou)

There is a few things I don't like about this.

First, it is very easy to punch in the wrong program number when I generate the nc code. Could I somehow set the program number from within Edgecam?

Second, it is a bit of a pain always transmitting 3 programs to the machine every time I switch jobs. (I store all programs on the PC, just transmit the programs as I use them) I suppose this is more of a machine side issue, I have Fanuc controls.

Third, I always must remember to put an M99 at the end of my subprograms, or else the machine will stop after the first subprogram. (or if I am testing each side individually and forget to take the M99 out, then the program will cycle right back to the beginning without stopping, which could be disastrous).

I would be interested to hear from other folks about how they are doing this, maybe there is a totally different and better way to do this. If I'm not making any sense, let me know and I will try to clarify.

Thanks a bunch!

[mystiks]

Kinda late perhaps, but i'll post this anyway, like to keep fresh mind myself =D. Dunno how old/new your machine is, so this might, or might not work.

Might be some serious typos here and there, or other problems aswell, wrote this after 14hour shift, bit tired.

For your 3 programs problem i'd like to suggest something similar that gildemeister type machines has (Program condition) . Something that can be easily done with some basic variables. Though i dont know if
your machine has this option avail, most have though. Think we have 2 older lathes that doesnt support macros at all, but anyway ->

You have your default "main" program which calls the 3phase program you'd like to use. Theres plenty of ways to do this, i'll just try to keep this simple and basic.




Main program:
-------------

O1000 (Main) ;

(P = Program used)
(A = Which phase to start out with)
(A0 = nopart / beginning)

G65 P5000 A#501

M30




........................




And you could use this as the default program tree where you copy+paste your 3 different programs. just renumber it for different parts 5001, 1001 whatever.

O5000 (Part name);
IF [#1 EQ 0] GOTO1
#501=#1
N1
IF [#501 EQ 0] GOTO5
IF [#501 GT 0] GOTO9
GOTO1001
N5
(INSERT NEW PART)
M0
#501=1
GOTO9
;
;
N9
IF [#501 EQ 1] GOTO10
IF [#501 EQ 2] GOTO20
IF [#501 EQ 3] GOTO30
GOTO1001 (ERROR 1)
;
;
N10
(PHASE 1)


Insert program 1 here


(FLIP PART)
M0
(FLIP PART)
#501=2
GOTO20
M30
;
;
N20
(PHASE 2)


Insert program 2 here


#501=3
GOTO30
M30
;
;
N30
(PHASE 3)


Insert program 3 here


#501=0
GOTO1



N1001 #3000=(Variable 1 must be 0-3)
M30
.
.
.

Im not sure if variable #501 is option or not, but i have used it on different fanuc mills/lathes/mx's and it has worked sofar, it should be a variable that saves over reset/machine turnoff so your current
phase doesnt clear from those actions. There are other ways to do this, and different ways to write macros but havent used too many macros yet, this should do the job though. You could add some variables to
do only certain phase, or start from phase 2 example if you have old half finished piece etc, the story is endless, just tried to make this simple.

Too tired to think of that G50(Is max rpm limiter on our machines), id use G10 to enter the right value on workshift.


On that program number from edgecam, should be doable, have to check from work though, cant postprocess anything from home yet.

[crazycnc]

Thanks for the ideas, mystiks. I also started this thread which you might find interesting as well. Thanks to all who participated, I have learned quite a bit about my machines that I didn't know!