[revlimit]

Hello everyone, we have an HRT 210 4th axis we rarely use. I need to plug this in and use it to repeat a simple milling pattern on a 10" diameter part every 15 degrees or so. My plan was to simply generate code for the milling pass then insert a command into the code to rotate the 4th axis 15 degrees, then repeat the milling procedure and so on. My problem is that I don't know what code to insert in to allow the 4th axis to turn. Thanks for any help you may provide!

[Stickerman]

Just put in G0 A15. to move it 15 degrees. You could make a subprogram to have it repeat enough times to machine all around the part.

[Stickerman]

You could do this...

After the tool change put this.

M97 P100 L24 (Call the sub 24 times)

(put all of your retracting moves here... coolant off or whatever)

M30

N100
G91 A15.
G90
(your main program)
M99

[Ydna]

You can use "A" codes inside a drill cycle. You also have the option of using G90/G91 for the angles too. Like this...
G81 X0 Y0 A0 (also need R,F,Z of course)
A15.
A30.
A45.
A60.
...

or use incremental...
G91 A15
A15
A15
A15
...

You might be able to use an L number to signify number of repeats, I can't remember if that works.

[revlimit]

Cooool! Thanks so much...I THINK I can take it from here. Looks good so far. Thanks guys!

[revlimit]

Hi again everyone, after refining the program, I end up with the need to rotate every 60 degrees instead of 15. I there a possibility that one of you (possibly Stickerman)can show me where to insert the data you've provided me? For example, I feel that I should insert:
"M97 P100 L6"
"M30"
"N100"
"G91 A15"
"G90" and finally,
"M99"........but I'm not 100 percent on exactly WHERE they should all fall in the mix. Thanks so much AGAIN for any help you guys may provide. Below is the current program I'm running now that is producing perfect parts....

%
O1234(slit,cbore,drill,tap6-1-2010)
N1G0G40G80G91G28Z0
T1M6(0.25,user_adjust_02500-00000)
G90G00G115X0.119Y-0.127S5200M3
G43Z2.0H1
Z1.0M8
Z.1
Z0.1
G85Z-0.25R0.1F8.32
G80
Z1.0
Y-0.521
Z0.1
G85Z-0.25R0.1F8.32
G80
Z1.0
G0Z2.0M9
G91G28Z0
M1
N2G0G40G80
T2M6(0.0781,center_2)
G90G00G115X0.119Y-0.127S5200M3
G43Z2.0H2
Z1.M8
Z-0.15
G81Z-0.373R-0.15F10.14
G80
Z1.0
Y-0.521
Z-0.15
G81Z-0.373R-0.15F10.14
G80
Z1.0
G0Z2.0M9
G91G28Z0
M1
N3G0G40G80
T3M6(0.136,TD_01360_29:J)
G90G00G115X0.119Y-0.127S5200M3
G43Z2.0H3
Z1.M8
Z-0.15
G83Z-0.4959Q0.205R-0.15F10.61
G80
Z1.0
Y-0.521
Z-0.15
G83Z-0.4959Q0.205R-0.15F10.61
G80
Z1.0
G0Z2.0M9
G91G28Z0
M1
N4G0G40G80
T4M6(0.12,TD_01200_31:J)
G90G00G115X0.119Y-0.127S5200M3
G43Z2.0H4
Z1.M8
Z-0.15
G83Z-0.7911Q0.26R-0.15F9.36
G80
Z1.0
Y-0.521
Z-0.15
G83Z-0.7911Q0.26R-0.15F9.36
G80
Z1.0
G0Z2.0M9
G91G28Z0
M1
N5G0G40G80
T5M6(2.75,2.75 slitting end mill)
G90G00G115X-0.8714Y1.8764S600M3
G43Z2.0H5
Z1.M8
Z-0.315
G1Z-0.416F100.0
X-1.195Y0.8616F20.0
Y-2.3468
G0Z1.0
X-0.8714Y1.8764
Z-0.315
G1Z-0.416F100.0
X-0.795Y1.2164F20.0
Y-2.3468
S500
F40.0
X-0.775Y1.2279
Y-2.3468
G0Z1.0
G0Z2.0M9
G91G28Z0
M1
N6G0G40G80
T6M6(0.138,tap#6-32 Form)
G90G00G115X0.119Y-0.127S1000M3
G43Z2.0H6
Z1.M8
Z-0.15
G84R-0.15Z-0.7547F31.25
G80
Z1.0
Y-0.521
Z-0.15
G84R-0.15Z-0.7547F31.25
G80
Z1.0
G91G28Z0M9
G91G28Y0
M30
%
THANK YOU!!!!

[Stickerman]

This is what I do when I have a program that's been written for a single part. Take the main part of each tool operation and put it as a sub. Just be sure to run this in the graphic view and don't trust anything I have done blindly since I know I can screw up anything!

I added a G90 and the starting X and Y coordinates in each subroutine and at the end there is a G91 A15. then a M99 so it will repeat the operation.

%
O1234(slit,cbore,drill,tap6-1-2010)
N1G0G40G80G91G28Z0
T1M6(0.25,user_adjust_02500-00000)
G90G00G115X0.119Y-0.127 A0 S5200M3
G43Z2.0H1
G97 P100 L24
G91G28Z0
M1
N2G0G40G80

T2M6(0.0781,center_2)
G90G00G115X0.119Y-0.127 A0 S5200M3
G43Z2.0H2
G97 P200 L24
G91G28Z0
M1
N3G0G40G80

T3M6(0.136,TD_01360_29:J)
G90G00G115X0.119Y-0.127 A0 S5200M3
G43Z2.0H3
G97 P300 L24
G91G28Z0
M1
N4G0G40G80

T4M6(0.12,TD_01200_31:J)
G90G00G115X0.119Y-0.127 A0 S5200M3
G43Z2.0H4
G97 P400 L24
G91G28Z0
M1
N5G0G40G80

T5M6(2.75,2.75 slitting end mill)
G90G00G115X-0.8714Y1.8764 A0 S600M3
G43Z2.0H5
G97 P500 L24
G91G28Z0
M1
N6G0G40G80

T6M6(0.138,tap#6-32 Form)
G90G00G115X0.119Y-0.127 A0 S1000M3
G43Z2.0H6
G97 P600 L24
G91G28Z0M9
G91G28Y0
M30

N100
G90 X0.119Y-0.127
Z1.0M8
Z.1
Z0.1
G85Z-0.25R0.1F8.32
G80
Z1.0
Y-0.521
Z0.1
G85Z-0.25R0.1F8.32
G80
Z1.0
G0Z2.0M9
G91 A15.
M99

N200
G90 X0.119 Y-0.127
Z1.M8
Z-0.15
G81Z-0.373R-0.15F10.14
G80
Z1.0
Y-0.521
Z-0.15
G81Z-0.373R-0.15F10.14
G80
Z1.0
G0Z2.0M9
G91 A15.
M99

N300
G90 X0.119 Y-0.127
Z1.M8
Z-0.15
G83Z-0.4959Q0.205R-0.15F10.61
G80
Z1.0
Y-0.521
Z-0.15
G83Z-0.4959Q0.205R-0.15F10.61
G80
Z1.0
G0Z2.0M9
G91 A15.
M99

N400
G90 X0.119 Y-0.127
Z1.M8
Z-0.15
G83Z-0.7911Q0.26R-0.15F9.36
G80
Z1.0
Y-0.521
Z-0.15
G83Z-0.7911Q0.26R-0.15F9.36
G80
Z1.0
G0Z2.0M9
G91 A15.
M99

N500
G90 X-0.8714 Y1.8764
Z1.M8
Z-0.315
G1Z-0.416F100.0
X-1.195Y0.8616F20.0
Y-2.3468
G0Z1.0
X-0.8714Y1.8764
Z-0.315
G1Z-0.416F100.0
X-0.795Y1.2164F20.0
Y-2.3468
S500
F40.0
X-0.775Y1.2279
Y-2.3468
G0Z1.0
G0Z2.0M9
G91 A15.
M99

N600
G90 X0.119 Y-0.127
Z1.M8
Z-0.15
G84R-0.15Z-0.7547F31.25
G80
Z1.0
Y-0.521
Z-0.15
G84R-0.15Z-0.7547F31.25
G80
Z1.0
G91 A15.
M99
%

[revlimit]

Stickerman, thanks so much. I've got a much better understanding of why the code is placed where it is now. Got a quick question on the "L" though. Is the "L" just a repeat value? For example L50 repeats a particular operation 50 times I assume? Also, I notice that the "P" and "N" values are incremented by 100..ex...P100, P200, N100, N200, etc. It seems that the N100 references the P100 and so on? One last thing, will this scenario run the parts through on the first tool then the second, third, etc.....or will it run one part then the second part, etc? Thanks again for your help!!

[Stickerman]

Yes, the L is how many times it repeats. The N100 could be N1 or N10 or whatever you want it to be. I started to do it with N1, N2, but then saw you had that in your other code and added the zeros.

The way I edited it the one tool would work all the way around the part then go to the next tool. It would be really simple to do it the other way, but would waste a bunch of time with tool changes.

[revlimit]

Stickerman, you're right, it certainly would waste a ton of time. I guess I was so focused on just getting it to happen that I wasn't thinking past the repeating. Thanks so much for the help. You guys are invaluable and I hope as time goes on I can contribute to solutions like these in return.

Gratefully yours,

J.Berto

[Geof]

When you use G91 for rotating the 4th axis you sometimes end up with it rotated several complete revolutions from zero. Haas has a feature called Quick Rotary G28 which lets you zero the 4th axis to the nearest zero point instead of 'unwinding' all the revolutions.

I cannot remember whether they are a Setting or Parameter that has to be turned on but I think there are two; one is called Quick rotary G28 and the other is Circle Wrap.

[revlimit]

Thanks Geof, I'll look into that at the end of the day when the operator has gone. We've been getting away with it because the end of the program contains optional stops that allow the operator to roll the 4th axis back around one position at a time. We need to do this to allow ease of part load/unload so it works well and we don't end up "wrapped." Thanks again everyone!

[revlimit]

Stickerman, the code in post 7 is giving me a bad g-code alarm. I'm assuming the G97's should be replaced with M97's. Going to try that. Thanks again!

[Stickerman]

Yep, M97 not G97... I said I could screw it up

[revlimit]

Works great now. You guys are great for taking the time to help out. Thanks again.