[MSGMachine]

I am having a little problem with a g83 peck drill cycle.I need to eather feed out of the hole or some how limit the rapid speed to 5% in the program before the canned cycle and turn it back to 100% after the canned cycle. Can one of you programming geniuses tell me if there is a way to do that.

Thanks

[Machineit]

I am having a little problem with a g83 peck drill cycle.I need to eather feed out of the hole or some how limit the rapid speed to 5% in the program before the canned cycle and turn it back to 100% after the canned cycle. Can one of you programming geniuses tell me if there is a way to do that.

Thanks

It would be good to explain why you need this.

Thanks-Mike

[Geof]

I do not know of any way to adjust the rapid rate from within a program and I have to admit it puzzles me why you want to do this. I guess if you have macros activated on your machine you could always write your own 'canned cycle' macro that would give you full control over everything. Without macros I think you will have to do it the hard way. Write a peck drill routine and put it in a subroutine then call this subroutine at every location you want to drill at.

[Delw]

I've had to do this on lathes never had a problem with mills( which I dont understand why) the reason I had to do it was due to chips building up and breaking the solid carbide drills I was using . I ended up long coding the program and used feed rates for the rapids and no canned cycles.

Geof
I always wondered if there was a way to adjust the g83 canned cycle to start feeding farther back from where the default is. isnt the default like .025 from the start of the last peck depth? ( I am not sure what the distance is just curious).

Delw

[Geof]

I can't recall anything about changing the rapid re-entry distance between pecks. The only adjustments I know about are the ones to reduce the peck increment as the hole goes deeper and the retract above R to provide better chip clearance and coolant entry into the hole.

[ToyMaker94566]

I've had to do this on lathes never had a problem with mills( which I dont understand why) the reason I had to do it was due to chips building up and breaking the solid carbide drills I was using . I ended up long coding the program and used feed rates for the rapids and no canned cycles.

Geof
I always wondered if there was a way to adjust the g83 canned cycle to start feeding farther back from where the default is. isnt the default like .025 from the start of the last peck depth? ( I am not sure what the distance is just curious).

Delw

What a trip this subject came up today, I'm in the exact same predicament. I'm drilling 3" deep stepping down in drill size every inch from .375 then .242 then .177 for the last inch using carbide drills in Nitronic 60. (Nasty stuff, work hardens instantly with cobalt drills.) Anyway, I've been M00ing before the deepest hole and manually lowering my rapid to 25% to give the chips a chance to get out of the way. I burned up a grand worth of tooling before I got it right; I still pucker with every cycle. And I thought I over bid this job, now I see why they gave it to me. :tired:

[ToyMaker94566]

I always wondered if there was a way to adjust the g83 canned cycle to start feeding farther back from where the default is. isnt the default like .025 from the start of the last peck depth? ( I am not sure what the distance is just curious).

Delw

Oh, and FYI, Yes there is a setting you can change. I was drilling some holes that were only .002 dia with pecks about .001 deep and backing off .025 was not acceptable. I called Haas and they told me which one to change. I'm sorry though, I forget which one it was. But there is a parameter you can tweak. Might find it in the manual.

[Donkey Hotey]

I'm still curious why you want the RETRACT speed to be slower. I can't see what this has to do with chip evacuation, cutter loads or anything else. Can somebody explain?

[MSGMachine]

The reason I am needing to do this is I am counterboring a very deep hole in ABS. sounds easy, but the chips what to wrap around the pilot of the counter bore cutter and melt easily, so I need the time to blow them off with coolant as the cutter leaves the hole.

I thought well, I will just retract further out. But I have to peck every .100 to get the chip control I need and it looks like torture on the z axis watching this thing rapid at 1000ipm in and out of this hole. And the hole is so deep I feel better slowing the retract and decent in and out of the hole.

5% rapid gives me the results I need, no problem. I just need this machine to run by itself and I don't want to leave the machine at 5% rapid loosing time for the rest of the program. (The rest of the program is lengthy.)

[Geof]

Delw

I had not read my manual carefully enough. Setting 22 adjusts the approach distance when pecking.

22 Can Cycle Delta Z
This setting specifies the distance the Z-axis is retracted to clear chips during a G73 canned cycle. The range is 0.0 to 29.9999 inches (0-760 mm).

[Donkey Hotey]

So--as Geof posted--extra retract height out of the hole won't solve your chip problem?

I wouldn't worry too much about the 1000 IPM rapids. If it bothers you, set the rapids for 50% which is still pretty darned fast. How many holes are you talking about per part? I don't think I'd worry about it if the 1000 IPM rapids are your root concern.

[Geof]

The reason I am needing to do this is I am counterboring a very deep hole in ABS. sounds easy, but the chips what to wrap around the pilot of the counter bore cutter and melt easily, so I need the time to blow them off with coolant as the cutter leaves the hole.....

I had a similar problem tapping Delrin with the chips wrapping on the tap. I finished up building an air blast nozzle operated by M21 that would come in to within half an inch of the tap and blow the chips off between holes.

Possibly what you could do is write the peck a sequence of G82 commands separated by a G04 pause with the R for succeeding G82s slightly less than the Z on the preceding one.

G82 Z-0.2 R0.01 (FIRST PECK)
G04 P10. (PAUSE 10 SECONDS TO CLEAR CHIPS)
G82 Z-0.4 R-0.19 (SECOND PECK)
etc

[Delw]

the plastic parts now that makes sence on why the slow retract feed, I always coded mine with individual peck moves using feed rates.

Geof,
I knew you would find something thanks, thats some good info to have.

amd your trick above would work perfect too.

[Matt@RFR]

I've never heard of anyone using an actual counterbore tool with pilot on a CNC machine. Can you instead use an endmill and helical interpolate the counterbore? That would solve all of your chip control issues, and I bet it would be much faster. Plus you'll have control of the counterbore diameter.

[ToyMaker94566]

I've never heard of anyone using an actual counterbore tool with pilot on a CNC machine. Can you instead use an endmill and helical interpolate the counterbore? That would solve all of your chip control issues, and I bet it would be much faster. Plus you'll have control of the counterbore diameter.

Agreed. But if the c'bore is that deep, I would have drilled it instead and then finished the last hundred thousands or so with the c'bore tool.

[Pondo]

If the C-bore is shallow, why not just chip break every .025 or less and not get long chips to begin with? (G73 Vs. G83)
I use an inserted carbide C-bore (for 3/8 SHCS) @1200 RPM, 12 IPM, and a G73 cycle with a chipbreak depth of .010" in tool steel (S7, H13, P20, etc.) for the same reason. Without the chipbreak, the chips wrap up bad. The Dia is about .61 and I go up to 1.5" deep with the cycle.

[Machineit]

If the C-bore is shallow, why not just chip break every .025 or less and not get long chips to begin with? (G73 Vs. G83)
I use an inserted carbide C-bore (for 3/8 SHCS) @1200 RPM, 12 IPM, and a G73 cycle with a chipbreak depth of .010" in tool steel (S7, H13, P20, etc.) for the same reason. Without the chipbreak, the chips wrap up bad. The Dia is about .61 and I go up to 1.5" deep with the cycle.

It's PLASTIC!