[Lene Madsen]

Hi Folks, I hope some of you can help me with this problem I'm having.

I'm trying to drill a 6 mm (63 mm deep, using a solid carbide drill) hole into a piece of steel that has been hardened to 60 HRC. My problem is the drills are breaking randomly, and my guess is that when using the G83 cycle the drill moves into the hole in rapid feed, which means if a little chip is stuck, on either the edge of the hole or on the drill itself, it will get dragged into the hole at rapid feed and thus breaking the drill.

I have tried to set the safe distance to 63mm meaning it would always start feeding above the hole, but my cam software tells me it would take several days to complete one hole (which I'm not really interested in :nono. I was adviced to run at 350 RPM and with a feed of 2 mm/min and pecks at ½ mm.

Any suggestions on how to stop breaking drills?


//Lene Madsen

[gunaydinemre]

hi I don' t know what kind of control do you use but if this is mazak you can use G73

N34 X30. Y674.5
N35 G43 G0 Z5. H25
N36 G73 X30. Y674.5 R5. Z-33.543 Q2. K17. D4.F440.

[meegers]

Hi guys,

See my attachments.

Sounds like you need to be using G73 on most Fanucs or Mazaks.

In Edgecam you'd select the Chipbreak cycle when drilling.

M

[Lene Madsen]

I'm using Fanuc 0MD on a Yang Eagle SMV 1000

I have looked in the manual and possibly I don't understand the G73. Can you explain it? As I read it this command does not withdraw the drill entirely from hole between each plunge?

My main concern is that the drill moves back into the hole in rapid feed, I would want to set a feed rate for moving down and then a smaller feedrate when actually drilling.


I appologize for my english, maybe I'm not explaining myself correctly.

[gunaydinemre]

for Fanuc
G21
G0 G90 G54
M3 S350
X100. Y50.
G43 Z100. H1
G98 (G99 Option) G83 Z-68. R1. Q0.5 F2.
X-100.
Y-50.
X100.
G80
G91 G28 Z0.
M30


if you use G99 code while tool is going new position to drill firtly (before new position)
tool must go up R position (Z=5) if you use G98 tool must go up G43 position (z100)

[henriktrolle]

Hej lene.

Jeg kan anbefale et bor fra Hoffmann varenummer 122305 som klarer 67 hrc det skulle du kunne køre 16 Vc med. og brug G83 og Q1 så skulle det gerne virke. husk at bruge den lave ildgang 5% eller hvad du har til rådighed.

m.v.h

henrik

[henriktrolle]

Prøv med 850 omdrejninger og en feed på 75

[Lene Madsen]

Henriktrolle, I will not be able to get to 63mm depth with that drill, but I was adviced to use 122536 which looks like to be just the longer version of that drill. The problem is that aldready 2 drills have broken using the G83 and I only make it to 20mm, how will it go at 60? I'm using much lower feeds and speeds but productivity is not my problem, I just want to make sure the drill makes it. Is it possible to go too slow?

[txcncman]

The clearance amount for the drill to rapid to before begin next infeed is set by parameter in your machine. You can also used a reduced rapid override during this drilling process, such as 25% (which also should be settable by parameter). If you want to feed into the hole at a different feed rate than the drilling feed rate, you will need to write the code for this. There would be several methods to achieve this code based on functions available on your machine.