Fanuc oT G83 deep hole drilling/reaming

anrapa · Oct 14, 2017

Hello!
I need to ream a hole that starts at z-20 (the first 20mm are already opened to a bigger diameter with a bigger drill bit) but I would like the reamer to travel back to Z5 each time instead of the beginning of the smaller hole (Z-20).
My lines are:

G0 X0
G0 Z-20
G98 G83 Z-40 Q1000 P2000 F0.05
G0Z5

This way the reamer does start at Z-20 but doesn’t go back to Z5 each time.

If I use G99 and add an R line the lathe does retract to Z5 but feeds at F0.05 FROM Z5 up to its next depth.

What I would like to do is to go rapid to Z5, then rapid to the previous max depth, feed for an additional mm, rapid at Z5, rapid at the new max depth, feed again and so on.

It doesn’t seem to be a way to do that, any clue?
Thanks a lot!
Tony

Inviato dal mio iPhone utilizzando Tapatalk Pro

brian.pallas · Oct 14, 2017

Some machines have "retract above R plane" setting. See if your machine has that and type in the appropriate distance. That is the easiest way I know of.

Other than that, I long handing doesn't take that long.

guest · Oct 14, 2017

Use G1. You shouldn't peck with a reamer anyway.

anrapa · Oct 14, 2017

It seems like my control doesn’t have the “retract above R plane” option, at least the manual doesn’t mention it.
The reason I’m peak reaming is that my reamer is a conical one (similar to a Morse Cone) and if I do it in one go it clogs and the brass or bronze parts melt (and the reamer snaps).

Inviato dal mio iPhone utilizzando Tapatalk Pro

guest · Oct 14, 2017

So in that case I would just add a couple more G83 lines, depending on how many swings you need take at the hole.

Just change the start point and Z depth on each canned cycle line.

anrapa · Oct 14, 2017

But if I start Deep I Can’t rapid out, that’s the problem

Inviato dal mio iPhone utilizzando Tapatalk Pro

guest · Oct 14, 2017

I think you have 2 options. Longhand the tool with G1/G0 or write a macro.

This would get more attention on the CNC forum. There are some other threads on the board on this topic.

I share your frustration. I use G74 cycles on deep holes, and deal with the same issue. I usually just split up the hole into multiple G74 cycles with different start points, but for tiny pecks and full retract on each peck it's a huge PITA.

anrapa · Oct 14, 2017

Yeah, manually writing code is what I normally do but I’m now experimenting with a different material and I’m trying to find the most efficient ratio between depth per pass. It can take a LONG time...

Inviato dal mio iPhone utilizzando Tapatalk Pro

guest · Oct 14, 2017

anrapa said:
...It can take a LONG time...

Problem with the approach is the deeper you go, the more the reamer engages with the part. What works on the first peck may not work on the last one. So you have to progressively get more conservative with the cut as you go.

I don't know the diameter you are working with, but I think I would try to ditch the reamer and go in with a miniature boring bar and a G71 cycle.

anrapa · Oct 14, 2017

That’s what I normally do with shorter parts but this particular part has a 3.7mm hole that opens to about 9mm over 60mm. I even had custom carbide boring bars made for me but they vibrate like crazy.

Inviato dal mio iPhone utilizzando Tapatalk Pro

guest · Oct 14, 2017

You're options are limited. If it was me, I'd be wanting to get that taper roughed out.

Step drill the hole with maybe 3 different drills, or rough it out with a 2 degree draft cutter. Get something in there with some chip clearance.

Then point to point with the reamer, at least you won't have a zillion tiny pecks to program.

anrapa · Oct 14, 2017

Yeah, at the moment I’m roughing it with 3.5 and 6mm drills, then a little with a 5mm boring bar up to Z-35 but then I have to do the reaming and this is when I need the peck rapiding out to Z3 so that the coolant can flush the stuff off the reamer while cooling it and the inside of the part.
But then I need a cycle that has to start outside the part and it takes 15 minutes with small increments when working on bronze.
Brass is fine, it takes 2 minutes in total, but bronze is so nasty and I can’t push the reamer that hard.

Inviato dal mio iPhone utilizzando Tapatalk Pro

DMF_TomB · Oct 15, 2017

on a mill G98 or G99 controls whether drill goes to initial Z or R value Z
.
i often use G98 Z2.0 and a R-2. (on separate lines of course) for a drill to go above part between holes but rapid into pilot hole down to -2.
.
not sure about lathe gcode read your manuals

anrapa · Oct 15, 2017

Yeah, that’s the code to avoid wasting time cutting air when the next hole is below the starting point of the previous. Unfortunately it doesn’t tell the machine to rapid out of the hole if you start deeper than the hole begins.

Inviato dal mio iPhone utilizzando Tapatalk Pro

DMF_TomB · Oct 15, 2017

anrapa said:
Yeah, that’s the code to avoid wasting time cutting air when the next hole is below the starting point of the previous. Unfortunately it doesn’t tell the machine to rapid out of the hole if you start deeper than the hole begins.

Inviato dal mio iPhone utilizzando Tapatalk Pro

.
G98 it rapids from initial Z to R value Z (which can be down deep into hole)but on a lathe the gcodes could be different i would look at the manuals for the machine usually where G83 is explained

anrapa · Oct 15, 2017

It rapids into it but when cutting it doesn’t rap it out to a specific and further distance, that’s my issue.
(It seems incredible to me that such a basic function isn’t part of every controller)

Inviato dal mio iPhone utilizzando Tapatalk Pro

screensnot · Oct 15, 2017

I wrote a macro for this. I don't have it in front of me, so I will try to re-type something close.

Drilling a hole that is already 20mm deep:

G0 X0
G65 P8083 Z-40. R5. Q1. D.5 I-20. F0.05 (Z=FINAL DEPTH, R=R-PLANE, Q=PECK, D=PECK CLEARANCE, I=INITIAL HOLE DEPTH, F=FEED)

____

O8083 (MACRO FOR DEEP HOLE DRILLING)
#100=#5003 (I-PLANE)
F#9
WHILE[#4GT#3]DO1
G0 Z#18
#4=#4-#17
IF[#4LT#3]THEN#4=#3
G0 G9 Z[#4+#17+#7]
G1 Z#4
END1
G0 Z#100
M99
%

edit: Verify first! I typed this from memory. Then shortly after, I edited a mistake.

DMF_TomB · Oct 16, 2017

anrapa said:
It rapids into it but when cutting it doesn’t rap it out to a specific and further distance, that’s my issue.
(It seems incredible to me that such a basic function isn’t part of every controller)

Inviato dal mio iPhone utilizzando Tapatalk Pro

.
.
i believe with a parameter change you can change how G83 operates with the rapid and feed. its possible it was changed to feed out on purpose
.
i have also changed before distance rapid stops from previous peck. often a chip is sticking up in the hole and if it slams into the chip at rapid it damages drill i have had to increase from 0.100 to 0.150" distance rapid stops and goes to feed over the last peck depth.
.
thats the trouble with CNC's in that parameter changes they can operate very differently. it can be good and bad at times. usually if i have a parameter book hardcopy i write in the book where setting is explained original setting and the new setting and when changed and name of who changed.

yardbird · Oct 16, 2017

This is what I use when do what you're wanting to do.

Brent

N70(MSG, 11/32" DRILL)
G0G99G40G54X14.Z10.T0
T0606

#1=.025(FEED SHORT OF)
#2=.070(PECK EVERY)
#3=.0(START DRILLING AND LOCAL VARIABLE)
#4=5.42(STOP DRILLING)
#5=.2(RAPID BACK SHORT OF)
#6=.0035(FEED RATE)

M41
G97S175M3
G0Z.3
G0X0M8
G0Z-[#3]
#3=[#3+#2]
N200
G1Z-[#3]F[#6]
G0Z.5
G0Z-[#3-#5]
G1Z-[#3-#1]F.2
#3=[#3+#2]
IF[#3LT#4]GOTO200
G1Z-[#4]F[#6]
G0Z.3
G0X8.
M9
G0G99G40G54X14.Z10.T0
M1

DMF_TomB · Oct 16, 2017

yardbird said:
This is what I use when do what you're wanting to do.

Brent

N70(MSG, 11/32" DRILL)
G0G99G40G54X14.Z10.T0
T0606

#1=.025(FEED SHORT OF)
#2=.070(PECK EVERY)
#3=.0(START DRILLING AND LOCAL VARIABLE)
#4=5.42(STOP DRILLING)
#5=.2(RAPID BACK SHORT OF)
#6=.0035(FEED RATE)

M41
G97S175M3
G0Z.3
G0X0M8
G0Z-[#3]
#3=[#3+#2]
N200
G1Z-[#3]F[#6]
G0Z.5
G0Z-[#3-#5]
G1Z-[#3-#1]F.2
#3=[#3+#2]
IF[#3LT#4]GOTO200
G1Z-[#4]F[#6]
G0Z.3
G0X8.
M9
G0G99G40G54X14.Z10.T0
M1

.
if he is using a CAM program which just uses G83, G73 or G81 it might be easier to read up on parameters effecting how it drills. parameter changes normally are easy to do, you just need to read or find out which ones. often their is a separate manual just on parameters
most changes require turning PWE on or parameter write enable on in mdi mode to change a parameter and to turn PWE back off when done. sometimes machine needs a restart.
.
i have also changed rapid feed rate from 500 to 200 ipm on Z axis. when drilling i didnt want it to go faster. other than the parameter was metric value it was easy to change the rapid feed rate too

Fanuc oT G83 deep hole drilling/reaming

Aluminum

Hot Rolled

guest

Guest

Aluminum

guest

Guest

Aluminum

guest

Guest

Aluminum

guest

Guest

Aluminum

guest

Guest

Aluminum

Diamond

Aluminum

Diamond

Aluminum

Hot Rolled

Diamond

Titanium

Diamond

Similar threads