Hi,
I have a deep hole which needs pecking to remove chips/swarf. I would like to keep the tip of the drill just inside the hole to prevent degrading the opening by multiple re-entries of spinning drill bit. Is this possible with g83 ?
TIA.
Printable View
Hi,
I have a deep hole which needs pecking to remove chips/swarf. I would like to keep the tip of the drill just inside the hole to prevent degrading the opening by multiple re-entries of spinning drill bit. Is this possible with g83 ?
TIA.
Use G73. (High Speed Peck) Fanuc and many others. (This will not retract to the top after each Q level, but only chip break)
That or you could drill a shallow hole to start using a standard G81, then change to G83 and make you R level a negative number.
G0X0.Y0.
G43Z0.1S2000M3
M8
G99G81Z-0.875R0.1F20.
G80
G0Z-0.5
G99G83Z-5.1R-0.5Q0.75F20.
G80
G0Z0.1 (CLEAR WORK PIECE)
M9
Thanks GG. Your second suggestion just occurred to me after posting. That fits the bill.
I was wondering whether it was possible to give R below but that will crash at G0. Two ops is the way to go .
Thanks.
Hi Reg, glad to help. Not that it matters much, but I'm pretty sure a G0 cancels any Fixed Cycle like G80 does. Meaning technically you wouldn't need the G80's. I just left them in there for good measure.
I want to keep clearance height, so I'd avoid a G0 between drillings and use G98. That makes an extra move but it's a rapid , so doesn't cost much.
G0 Z5 (CLEAR CLAMPS)
S2000M3
G98
G81 Z-0.875 R0.1 F20 (Rapid to 0.1, drill pilot, G98 RETRACTS TO PREV Z : 5)
G83 Z-5.1 R-0.5 Q0.75 (WHEN DONE, RETRACTS TO PREV Z : 5)
G80
That seems to do what I want.
thanks for your suggestions, it helps me know I'm not missing some obvious move in one command.
Hi Reg, Yes nice going using G98. I canceled and put that Z move in there (originally included X0.Y0. but dropped it) because the machine will likely not do the 2nd half of your routine without a location call. You'd have to try it and see but it might not do two routines in a row at the same location without something in between.
Let me know if it works as is. Curious.
Thanks I'll test it when I get a chance.
Why would the machine not do what I told it? Are there "smart" Gcode interpreters which think they know better and refuse to follow gocde instructions ?
The A: is that gcode is endlessly complex with endless variations, implemented in endless ways by various companies.
Legal gcode can be interpreted quite differently by 2 different controllers, or variations of the same controller, and both be "right".
Gcode is not properly defined, and subs and macros are not really defined -- more like this is how it used to work.
Quote:
Originally Posted by reg.miller
Hi Reg,
I just had to make a test when I got in this morning. Ran something very similar to your G98 suggestion. Worked perfectly fine, as I think it would on any machine. At least a Fanuc one. I tested it on my OMC.
I think my double position call idea came from a trick I have to use on my non Rigid Tapping OM. I play a game so it doesn't shift into the reduction gears as it normally does for anything under 1200rpm. This makes the response time of the spindle on and off much better, as it's not having to go thru a 4:1 reduction gear set. It's something like I call a tapping cycle with the machine already in the XY position, but no Spindle speed stated. I then give it an S value sort of after the fact. If I don't recall the position it just sits there and does nothing. That or it moves to the next hole before it does anything.
Long story... sorry. Anyway... in a normal world, telling the control to double cycle a hole works just fine. :-)
G00, G01, G02 and G03 all belong to the movement group of codes and will turn off any active canned cycles, not recommended though.Quote:
Originally Posted by the_gentlegiant
It is not good practice to turn off your canned cycles using movement codes.
Always make it clear that canned cycles have been turned off by using the G80 cancel command once you have finished running your canned cycles, another reason it should always be in the Program Header (Safety Line) also.
Already standard practice here.Quote:
Originally Posted by mactec54
Every tool I've ever called starts out like this: (Obviously changes to start location/H/T/S and sometimes G54 needed)
T2M6 (A TOOL OF SOME KIND)
G17G20G40G49G54G80G90G98
G0X0.5Y-0.5
G43Z0.1H2S7500M3T3
M8
The Safety Line is not effective when you are running through a program, a G80 must be used, or it can reuse the active Canned cycle after a move to another position.Quote:
Originally Posted by the_gentlegiant
The Safety Line is in effect only at the start of a Program and cancels all previous calls that may not have been canceled.
Guess I wasn't understood earlier.Quote:
Originally Posted by mactec54
I always use G80 to end Fixed Cycles. My Safety Line only only adds to the certainty of the machine's condition at the start of a new tool. No matter what happened before it.
It may also have been missed that the programming example I gave in post #11 is how every tool starts in a program, not how every program starts. (Except for the fact that eventually, every program starts with a tool loading to the spindle.) It's super redundant, but I also use it as a tool start header, because it's easy to spot when scrolling through a program. I program semi manually, meaning no post processor is spitting out my code sight unseen, so quickly finding tool startups is important to me. The two distinct looking lines with the space right after really helps.
Earlier I only mentioned how G0 will cancel a Fixed Cycle as simply stating a matter of fact. Not that I was advocating for it in general use.