Results 1 to 8 of 8
Thread: Haas VF1 peck drilling trouble

04032019, 06:20 AM #1
Haas VF1 peck drilling trouble
So I am new to a Haas machine and I recently purchased a 2000 Haas VF1. I am having trouble with peck drilling with G83 in that the machine errors with "Invalid I, j, k". In the book it calls I, J, and K commands optional and I have omitted them as I don't wish to use them at this time.
This is my code section, it errors/stops after the first hole drill. Suggestions?
Code:G83 X0.7385 Y0.4375 Z0.625 Q0.21 R0.125 F20.0 G83 X0.7235 Y2.1875 Z0.625 G83 X3.2765 Y2.0995 Z0.625 G83 X4.7235 Y2.1875 Z0.625 G83 X4.7385 Y0.4375 Z0.625 G83 X3.2615 Y0.5255 Z0.625 G83 X7.2615 Z0.625 G83 X8.7385 Y0.4375 Z0.625 G83 X8.7235 Y2.1875 Z0.625 G83 X7.2765 Y2.0995 Z0.625 G83 X11.2765 Z0.625 G83 X11.2615 Y0.5255 Z0.625


04032019, 06:46 AM #2
I just posted some code to drill holes in a part for my HAAS VF2 take a look and see if this helps. You should only need to call the G83 on the first line and cancel it at the end using a G80
N100 G20
N110 G0 G17 G40 G49 G80 G90
N120 T3 M6
N130 G0 G90 G54 X17. Y3.25 S2439 M3
N140 G43 H3 Z.1
N150 M8
N160 G99 G83 Z.625 R.1 Q.1 F6.
N170 X15. Y.38
N180 X3.
N190 X1. Y3.25
N200 X3. Y6.13
N210 X15.
N220 G80
N230 M5
N240 G91 G28 Z0. M9
N250 G28 X0. Y0.
N260 M30
%
Good luck
Make Chips Boys !
Ron

04032019, 06:53 AM #3
That's some messy code.
G83 is modal and stays in effect until cancelled by G80. Could be the problem.
Either add G80 in between every G83 line or delete all G83 except the first one. You could then delete all the Z.625 as they're redundant.

04032019, 07:41 AM #4
Thanks for the help. That fixed it.
This code was created with cambam so I need to figure out how to edit the post processor to make this correct code. I am now doing everything with Fusion 360, but these older designs were already completed with cambam and I need to get them running again on the new mill asap.
Code:% O2002 ( SMART100.1_031919_CAM 4/3/2019 8:10:30 AM ) ( T5 : 0.0625 ) G54 G20 G90 G64 G40 G0 Z0.125 ( T5 : 0.0625 ) T5 M6 G43 H5 ( DRILL1 ) G17 M3 S5000 G0 X0.7385 Y0.4375 G99 G83 X0.7385 Y0.4375 Z0.625 Q0.21 R0.125 F20.0 X0.7235 Y2.1875 X3.2765 Y2.0995 X4.7235 Y2.1875 X4.7385 Y0.4375 X3.2615 Y0.5255 X7.2615 X8.7385 Y0.4375 X8.7235 Y2.1875 X7.2765 Y2.0995 X11.2765 X11.2615 Y0.5255 G80 G0 Z0.125 M5 M30 %

04032019, 02:14 PM #5
OK, so your problem was as follows:
the G83 block MUST have either I, J, K, OR a Q value.
These values are nonmodal, meaning after the block is cancelled ( either by G80 or any other group command ), they are erased and must be redefined for the next G83 call.
In your case your post called the entire G83 cycle for each and every hole. While that is completely unnecessary, it also cancelled the previous G83 definition
and recalled it, but now without the Q definition.
Basically your code was equivalent to:
G83 X0.7385 Y0.4375 Z0.625 Q0.21 R0.125 F20.0
G80
G83 X0.7235 Y2.1875 Z0.625
G80
G83 X3.2765 Y2.0995 Z0.625
G80
G83 X4.7235 Y2.1875 Z0.625
G80
G83 X4.7385 Y0.4375 Z0.625
etc....
Note that any G83 block after the first one are missing the Q value.
R can be omitted as it can come either from the block's definition, or if omitted there is a default in the Settings page.
F is modal, so it sticks
P can be omitted, and if so it's assumed to be 0
I,J and K OR the Q value however is mandatory, so one or the other MUST BE EXPLICITLY DEFINED IN EACH G83 call!

ForcedFour liked this post


04032019, 03:57 PM #6
That makes perfect sense. Thank you!
I added the R value because after getting it to work as above without the R value the spindle would rapid all the way up to Machine Z0 after each hole drilled. Likely a setting would fix that, but adding the R value also fixed it and got me machining today.

04032019, 04:04 PM #7
That's because you have no initial plane. If you said G43 H5 Z1.0, the retract would go to Z1.0.
Since there is no Z position prior to reading the G83 line, it goes back to the starting point which is Z home.
G99 is retract to R plane, so adding the R plane means it will rapid to R and retract to R for the duration of the G83 cycle.

rklopp liked this post

04042019, 08:22 AM #8
If your holes are all the same, then all you need after the first G83 call out is the next location. For example: X4.7235 Y2.1875. When you call out the G83 again, it needs the Q and the R again.
G83 X0.7385 Y0.4375 Z0.625 Q0.21 R0.125 F20.0
X0.7235 Y2.1875
X3.2765 Y2.0995
X4.7235 Y2.1875
X4.7385 Y0.4375
X3.2615 Y0.5255
X7.2615
X8.7385 Y0.4375
X8.7235 Y2.1875
X7.2765 Y2.0995
X11.2765
X11.2615 Y0.5255
Bookmarks