Need some help people, currently programming HAAS ST35Y. I am using the G112 function for milling a series of arcs and lines around my billet, I use G112 because I can program it in X and Y and the control will convert it to C using polar. It's milled my shape no problem, but when I move away to clearance in Z and X and call off that function with G113 the machine decided to send my tool back towards my workpiece and if I allow it to do what it wants it will plunge in to the job. Any ideas what's happening here?
Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
Z axis movement when Canceling Cartesian To Polar Transformation G112-G113
- Thread starter Donny092
- Start date
- Replies 11
- Views 1,664
Ox
Diamond
- Joined
- Aug 27, 2002
- Location
- Northwest Ohio
Post the code.
--------------
Think Snow Eh!
Ox
--------------
Think Snow Eh!
Ox
The start of my Block is:
G0 Z3.
G0 C0.
M08
G112
G0 X50.
G1 G42 Z-7.4 D09 F150.
Then it machines my profile out perfectly.
So I end my Polar portion of the process as :
G0 G40 Z10.
G113
(Here is where it wants to travel back in to my work piece)
G0 G55 G17 G40 G80 G98
G0 X18.6
G0 Z3.0
G01 Z-3.5 F250.
G13 I8. Z-3.5 F350. D09
I think it maybe something to do with Tool Comp. Maybe I need to cancel it on a feed rather than a rapid or something, We all know how much of a headache tool comp can be!
Ox
Diamond
- Joined
- Aug 27, 2002
- Location
- Northwest Ohio
I don't doo a lot of C werk anymore (thankfully to Y) but looking back at a good program for a Fanuc, the only thing that I see is that I "fed" off the part at like 200 IPM and then fired the G113, before calling a G0, but I have no clue why that would make any difference?
You already canceled your comp in the previous line (and the next one as well? - good to be sure I guess... LOL!) so I don't expect that is the culprit.
Mine is Fanuc, and I never ran a Haas, so there could be a small difference there.
???
-------------------------------
Think Snow Eh!
Ox
You already canceled your comp in the previous line (and the next one as well? - good to be sure I guess... LOL!) so I don't expect that is the culprit.
Mine is Fanuc, and I never ran a Haas, so there could be a small difference there.
???
-------------------------------
Think Snow Eh!
Ox
TeachMePlease
Diamond
- Joined
- Feb 11, 2014
- Location
- FL
Is the tool rapiding into the workpiece in X I assume?
Figured it out, turns out you have to be at your Z depth when you cancel the command, I was moving away in Z and X to my next start position and then cancelling the command. It was going back to its Z depth to cancel it, I moved away to clear the job in X axis and kept it at its Z depth, then canceled the command and moved away in Z axis after, which seemed to sort I out.
GENERALDISARRAY
Hot Rolled
- Joined
- Jan 3, 2019
G0 during polar?
Ox
Diamond
- Joined
- Aug 27, 2002
- Location
- Northwest Ohio
Yeah, I'm thinking that G0 in Polar is a no-no in Fanuc too.
At least my code seems to point to that.
Maybe you should try to move off in G1 F200. and then cancel and see how it responds - just for the sake of understanding.
-------------
Think Snow Eh!
Ox
DouglasJRizzo
Titanium
- Joined
- Jun 7, 2011
- Location
- Ramsey, NJ.
On Fanuc, rapid moves in Polar mode are usually not allowed. So I always taught that you did a "fast feed" - in this case, a "G1 G98 Z.25 F120." to retract the Z, then go onward. When cancelling, a G13.1 (or G113 depending) after a G1 move is the way I did it.
coyoinu
Aluminum
- Joined
- Oct 6, 2012
- Location
- Orange county, CA
please send me your full program, i'd really like to take a close look at that.
angelw
Diamond
- Joined
- Sep 10, 2010
- Location
- Victoria Australia
Hello Donny,
I know its the case with Fanuc and it states specifically in the Haas Manual that "Z-axis moves are not allowed while this mode is enabled" (extract from manual). Accordingly, the "Z" move in your following code is also incorrect:
G112
G0 X50.
G1 G42 Z-7.4 D09 F150.
Regards,
Bill
DouglasJRizzo
Titanium
- Joined
- Jun 7, 2011
- Location
- Ramsey, NJ.
PM me if you need.
