What's new
What's new

How do you do a coordinate shift with a Brother C00 control, and other questions

DavidScott

Diamond
Joined
Jul 11, 2012
Location
Washington
I am changing an old program to run on my new Brother and can't figure out how to shift the coordinates on it. The code I use on my Yasnac is G52Q2Y amount, or G10 would work. I need to shift the Y axis 8 times calling a sub after each shift in the extended workpiece coordinates. How do you do a coordinate shift with a Brother C00 control?

Also while I am asking questions how do I code the extended workpiece coordinates? I "think" it is G54.1P2 etc. G54.1 enables and P2 selects which level, 2 being the first extended level. Clarification would be nice, please. I am hoping to start making paying parts tomorrow, the first for this machine since I got it over a month ago so kinda excited.
 
Extended work offsets:

G54.1 P1
G54.1 P2
etc.



In my opinion, workshift is easiest with G52. In your case, assuming a 2" shift each time:

G52 Y0. (zero workshift for your first position)
Sub Call
G52 Y2. (shifts Y +2")
Sub Call
G52 Y4. (shifts Y another +2")
Sub Call
etc.

And then G52 Y0. when done. If you're screwing around with workshifts like this, I find it's a good idea to include another safety line in your standard header like this:

G52 X0. Y0. Z0. Just for cuz.
 
Thank you, the manual says a G92 will cancel G52, or cycle reset. I shift the coords on the last tool of the second, and last, op.

Do you know how to control the reducing value when peck drilling?

And is there a way to have the head move in all 3 axis after the tool change? Mine positions X and Y while changing the tool, then once X and Y are positioned it moves Z. I am wondering if there is a parameter that controls how the machines handles G100 movements.
 
Thank you, the manual says a G92 will cancel G52, or cycle reset. I shift the coords on the last tool of the second, and last, op.

Yes, several ways to cancel G52, but the only way I trust is to cancel it myself with a G52 X0. (or Y or Z or all three).
Do you know how to control the reducing value when peck drilling?

I hand program any drill cycles that require anything other than a regular peck, so not sure about that your reducing-peck question.
And is there a way to have the head move in all 3 axis after the tool change? Mine positions X and Y while changing the tool, then once X and Y are positioned it moves Z. I am wondering if there is a parameter that controls how the machines handles G100 movements.

Are we talking about an R or an S machine? I'm assuming S since it would be a very bad idea to move Z during G100 as the pallet rotates. I don't have an S machine, so no help there.
 
R650 and I haven't got to rotating the pallet while changing a tool yet, hopefully tomorrow. Yes bad when rotating a pallet, but good on all other tool changes, barring any obstacles.

On Fanuc or Yasnac you control your peck drilling with i, j, and k. Brother uses W and V for i and k but does not provide the equivalent of j. It seems the reduction value is automatically 20% of W.
 
R650 and I haven't got to rotating the pallet while changing a tool yet, hopefully tomorrow. Yes bad when rotating a pallet, but good on all other tool changes, barring any obstacles.
I get the feeling you haven't run this thing at 100% yet. It will position X and Y during all tool changes using G100, obviously it can't move in Z until the tool change is done. I guess I haven't watched ours all that closely, but I'm pretty sure any X/Y move is going to be finished before the tool change is finished, or close enough that it doesn't matter if you end up getting an actual 3 axis move after the tool change or not. You are splitting hairs that don't need to be split yet. Just get used to the thing for a month or two (at 100%) and then start going after time savings if you really have the need to.

One thing I did was to use a modified tool breakage program that doesn't home the Z. Risky, but it does save time. Not a lot, but some. I am not going to post that here. If you don't know how to modify the existing cycle, then you're not ready to be taking risks like that anyway.

People told me this and I didn't believe them until I really got in the weeds of killing cycle time on long runs: These things are so fucking fast that you can spend hours or days hand tweaking a program with no air time, no retracts, High Accuracy codes all over the place, be all proud of yourself, run the program and save 3 seconds of cycle time. You can be sloppy with Brother programs and not be hurt bad at all, time wise.
 
Last edited:
People told me this and I didn't believe them until I really got in the weeds of killing cycle time on long runs: These things are so fucking fast that you can spend hours or days hand tweaking a program with no air time, no retracts, High Accuracy codes all over the place, be all proud of yourself, run the program and save 3 seconds of cycle time. You can be sloppy with Brother programs and not be hurt bad at all, time wise.

Aside from the obvious palaces everyone turns to to find time - lead in/out reduction, minimize retractions, none of this business where the drill starts half an inch above making contact with the material - the two places to find time in a Speedio are:

1- Using G100 properly. The number of times I see a tool retract, stop, coolant turns off, spindle turns off, then it accelerates back up to change. Conversely, tools that stop on approach to set offsets, turn on coolant, etc etc. G100 handles everything and to work properly, you need to let it. As soon as the tool comes out of contact with the material? G100 to the next tool - don't even retract to the operation clearance plane, just go. No fiddle fucking with G40 or coolant off codes. Let G100 do what G100 does. Also, call all the stuff you would do on approach in G100 - coolant, G43, work offset.
So many people are giving up at least a second on their total tool-change cycle by not using G100 properly.

2- High Accuracy modes. I recently got schooled by an old project that I worked on that the customer had put on the back shelf due to COVID. They came back to it and had their excellent inside guy program it, but they still wanted a bit more time. Compared notes, got the latest code (with no HA applied), added my usual M298 bits where I would normally put them and... My code was like 30 seconds slower on a ~2 min cycle. WTF?
Turns out, they were just using the M298 Roughing for *everything*, save critical profiles which used Finish. All my fussy accuracy setting and thoughts about what was necessary? Totally out the window, I never even thought about trying the whole thing in Rough and seeing what would happen. Lesson learned - on jobs where you are really dialing in, throw away your standard High Accuracy defaults and work backwards. Default to keeping everything wide open, then selectively apply the minimum HA code required to bring the part into the desired results.
 
I use G52 for all my coordinate shifts. Have G54 set for my standard 'zero' then shift from there.
G52 is, I think modal, so it never bites me by having it stay at some odd shift and crashing into stuff[at least so far]
I put them in a subroutine so that when I am drilling tapping countersinking between vise stops there is but one number to change to dial in the part.
 








 
Back
Top