Can you Peck + Chip break in Brother Speedio?

[Finegrain]

Hello,

Without programming separate toolpaths, is there a way in a Brother Speedio to add chip break to a peck drill cycle?

Thanks, and regards.

Mike

 

[DavidScott]

As in G83 or G73?

Not sure what you are talking about.

 

[Finegrain]

As in G83 or G73?

Not sure what you are talking about.

G83 pecks by Q value, with a full retract between pecks. For getting coolant down into deeper holes.
G73 retracts a tiny bit every Q value, but never fully retracts. For preventing bird's nests around the drill.

I want a cycle that does both -- no bird's nests, and full retract occasionally to get coolant down into the hole.

Regards.

Mike

 

[TeachMePlease]

You should be able to bang out a macro for it fairly quickly.

 

[gustafson]

HOw deep are you going?
IT is so fast the amount of time you are going to save in the difference between the two is fractions of a second.
While I am annoyed by the lack of many cycles in the brother, you can call an internal sub program that is the series of Z moves you wish pretty easily.

Making it an external sub program would enable you to easily copy and paste it to a new sub and change the depths.
I do this with my back burring programs with very little trouble.
As mentioned you can write a macro but you need dozens of different hole depths and many thousands of holes to make up the time required to even think about it.
i know heidenhain has a decrementing drill cycle, but again, the brother is a little limited in this regard

 

[Booze Daily]

String a couple G83’s together with deeper Z’s and deeper R’s?

 

[LOTT]

I can spec that in Fusion, to include the peck depth and retract intervals, and it post a bunch of G1's and G0's. It's inelegant and bulky, but the Brother inhales code and has plenty of memory so who cares....

 

[yardbird]

You might be able to get away with just dwelling a short bit instead of actually pecking or pulling out any. I might trying mixing absolute and incremental programming. Repeating the pecking portions by calling a sub, retracting out completely at whatever absolute Z- distances of your choosing. Calling a sub would make editing the pecking routine portion easier. I say this without knowing anything about the Brother control or the kind of depth you're talking about.

Brent

 

[gkoenig]

Why are you drilling with canned cycles? They are a leftover from hand programming days - output raw G01/G00 motion and be done with it.

 

[sinha]

String a couple G83’s together with deeper Z’s and deeper R’s?

G73 actually, with G98.

 

[Finegrain]

Why are you drilling with canned cycles? They are a leftover from hand programming days - output raw G01/G00 motion and be done with it.

My POST only outputs canned cycles.

Greg, you saw what sort of work I have these days. Quantity dozens, sometimes hundreds, but lots of different parts every week. I need my CAM to output code as close to finished as possible. If you know of a MasterCAM POST that has more subtle drill code than G73/G83, I'd be happy to try it out.

Regards.

Mike

 

[TKassoc]

You can go into the Control Definition and change the output to post longhand drilling cycles with one checkbox. Control Definition-->Machine Cycles-->Mill Drill Cycles and uncheck any of the ones you don't want output as canned cycles

 

[dodgin]

My POST only outputs canned cycles.

Greg, you saw what sort of work I have these days. Quantity dozens, sometimes hundreds, but lots of different parts every week. I need my CAM to output code as close to finished as possible. If you know of a MasterCAM POST that has more subtle drill code than G73/G83, I'd be happy to try it out.

Regards.

Mike

I'm curious, does this include the advanced drilling path? Because that could work well for you if the post isn't in the way.

 

[gkoenig]

Greg, you saw what sort of work I have these days. Quantity dozens, sometimes hundreds, but lots of different parts every week. I need my CAM to output code as close to finished as possible. If you know of a MasterCAM POST that has more subtle drill code than G73/G83, I'd be happy to try it out.

TK has you covered above, and you'll love it. Total control over the drilling cycle!

Literally the only thing I use canned cycles for anymore is G77 Tapping, since I don't believe there is any other way to synchronize spindle motion and feed (I think there may be, but haven't looked too deeply into it).

 

[couch]

I am annoyed by the lack of many cycles in the brother

Which cycles are you missing?

 

[gustafson]

Which cycles are you missing?

most of them

Seriously, this machine is not meant to be programmed at the machine, even though I do a fair bit of it, so it is a bit of a peeve for me.
No pocketing cycles for instance.
No thread milling cycle.

 

[DavidScott]

Which cycles are you missing?

No programmable reducing value for G83, this is REALLY limiting. The canned cycle for thread milling looks interesting, although I haven't used it.

 

[Volitan]

My POST only outputs canned cycles.

Greg, you saw what sort of work I have these days. Quantity dozens, sometimes hundreds, but lots of different parts every week. I need my CAM to output code as close to finished as possible. If you know of a MasterCAM POST that has more subtle drill code than G73/G83, I'd be happy to try it out.

Regards.

Mike

Are you current with your maintenance? They just added this recenty. It's maybe in 2021? You can have I think 10 different peck amounts or something like that. Haven't played with it but it's in there. All in G1's and G0's.

 

[Volitan]

Why are you drilling with canned cycles? They are a leftover from hand programming days - output raw G01/G00 motion and be done with it.

If you don't need to do anything fancy like change peck increments, is there an advantage to straight motion programming vs. canned cycle?

 

[couch]

No programmable reducing value for G83, this is REALLY limiting. The canned cycle for thread milling looks interesting, although I haven't used it.