Incremental circle milling sub program

[Diggs]

This should be an easy question for some of you but I had a hard time today writing a short sub-program trying to rough mill a 1/2" hole to .950 in a hole pattern. We have a new VMC but haven't chosen a CAM package yet so it is finger cam for now and I have not done alot of this. I want it to use cutter comp, have 2 depths of cut (.500 each), and be incremental(so I can go to the locations and run the sub). I was using a 1/2 rough mill in 304SS. I could do it without cutter comp no problem, but I want cutter comp. I was either on the wrong side of the cut, or it wasn't making a full circle, or just wouldn't compute(error). It was driving me nuts. I was trying to use g41 and g03 for cutter comp left and counter clockwise rotation (climb milling) but I finally gave up. I finished writing it without cutter comp and will run it tommarrow unless someone here can enlighten me. Any help would be greatly appreciated.

[gar]

080103-2016 EST USA

Diggs:

If you have a HAAS machine and it is in Fanuc or HAAS mode, then you can use G52 to create a child coordinate system relative to your current G5x base. Doing this you can work in absolute instead of incremental. Since HAAS in either of these modes is a derivative of Fanuc you should be able to do the same thing in Fanuc.

.

[Diggs]

G52 to create a child coordinate system? hmmm sounds interesting, I'll have to consult the manual about that. I am using a Fanuc Oi.

[cnc-king]

check this thread out some interesting info here on milling a hole

http://www.cnczone.com/forums/showthread.php?t=46754

[psychomill]

An incremental sub with comp shouldn't be a problem though... without having to resort to using G52. Post your code Diggs.... Let's see what you've got...

[Geof]

[QUOTE=psychomill;388344... without having to resort to using G52...[/QUOTE]

Whadda ya mean? "resort to"? For us enlightened ones G52 is the preferred choice.

[psychomill]

I knew that would get someone's attention... either you or GAR...

All kidding aside, there's no reason why what he's doing won't work. I use to do it all the time... Then I might shift the entire operation by G52 while using incremental subs.... but thats another story. Just curious to see his posted code since it should work.... just may not be picking up something correctly..

[Diggs]

OK, I already made the parts without cutter comp using something to the effect of:

G01X-.225Y0
G03I.225

I had already trashed my program I was attempting yesterday but today I was trying something else today afterwards and getting errors again whenever I tried to introduce cutter comp. Here is what I have that works without the G41 & D5(but cuts .500 too big obviously). I go to the position over the .500 hole and M98 P7001;

:7001
(CIRCULAR HOLE SUB)
N010G90Z.1
N020G01Z-.463F10
N030G03G91X.475Y0R.2375F4
N040G03I-.475
N050G03X-.475Y0R.2375

this is just the beginning of sub but far enough to go no further.

If I put the G41D5 in the first G03 line I get an error:
034 NO CIRC ALLOWED IN ST-UP /EXT BLK

If I put it in the G01Z move above it, I get the error:
020 OVER TOLERANCE OF RADIUS ERROR

These are the same gdamn errors I was getting yesterday using all X,Y,I,J in the G03 lines

[Geof]

Originally Posted by Diggs If I put the G41D5 in the first G03 line I get an error: 034 NO CIRC ALLOWED IN ST-UP /EXT BLK(

As far as I am aware you are not allowed to set tool comp, G41 or G42, on an interpolated move only on a G00 or G01.


With the tool in position over the hole and Z zero at the surface of the part my code would be;

G91G41D05G00Y0.475Z0.0
G03I0.J-0.0475Z-0.05F(whatever)L10
G03I0.0J-0.475L2
G40G01Y-0.475
G90G00Z1.0

This code might leave a witness mark because the G01 to cancel comp has the cutter stopping and then moving away on a radial line. To avoid this you could use;

G91G41D05G00Y0.475Z0.0
G03I0.J-0.0475Z-0.05F(whatever)L10
G03I0.0J-0.475L2
G03X0.0Y-0.9I0.0J-0.45
G40G01Y0.425
G90G00Z1.0

This has the cutter moving away on a smaller circle tangent to the bore before the tool comp cancellation so it does not come to a full stop in contact with the work.

I think my numbers are correct, I haven't run this through my simulator.

[Diggs]

I just tried those and both were similar in that the first circle was above the hole and the others was correct(around the hole). I ran them to scratch cut a piece of aluminum, and they gave me a figure eight pattern with a little ramping in. I also had to take out that G00 in the first line or it would have rapided into the material had I been in the hole.

I am leaving work now so I wont be able to try anything till monday.

I appreciate the efforts though. We'll (I'll) get it eventually. thanks

[Geof]

I have to hang my head in shame and apologise I was way too sloppy with some J-0.0475s which should have been J-0.475 and other things not quite correct.

This below does work on my Haas; one hole located at the G54 work zero, one 2 inches away, both using incremental for the hole. First hole does the radial entry and exit and second hole does the tangential exit before cancelling tool comp.

I hope I have redeemed myself.

%
O00000
G17 G20 G40 G49 G80 G90 G98
G10 L12 G90 P5 R0.5
T5 M06
G43 H05
M03 S10000
G90 G54 G00 X0. Y0. Z1.
Z0.01 M08
G91 G41 D05 G00 Y0.475 Z0.
G03 I0. J-0.475 Z-0.051 F100. L10
G03 I0. J-0.475 L2
G40 G01 Y-0.475
G90 G00 Z1.
G90 G54 G00 X-2. Y0.
Z0.01
G91 G41 D05 G00 Y0.475 Z0.
G03 I0. J-0.475 Z-0.051 F100. L10
G03 I0. J-0.475 L2
G03 X0. Y-0.9 I0. J-0.45
G40 G01 Y0.425
G90 G00 Z1.
M30
%

[Diggs]

Well I will be sure to give it a try and reply back as soon as I do. Most likely I will have to do some actual work during the first part of next week before I can find some time to "figure stuff out" but I will asap. Your efforts are much appreciated.