Work Coordinates and Offsets for repeat jobs

I am setting up my first "production" job that will be a repeat in my shop. I've been a tool maker my whole life and while I have worked in some BIG production facilities, I avoided the production side like the plague.

A little bit of an outline of the job, then a few questions about opinion on setup.

Job as I have it setup was going to be 5 work coordinates. I decided to condense the last three setups into a fixture, which I *hope* will work. Going to cut it and try it out today. This seems like a simpler approach to cutting 3 sets of soft jaws. If everything goes to plan I will make two of the fixtures so I can pull one out to do my changeover while the other is running.

I am trying to be proactive for this job because it should re run in a few months (3-6mo) The job is small, 60pcs, but the parts are fairly high complexity with several features that are close tolerance, and several "aesthetic" requirements.

My question in relation to the fixture. As I program the parts, I am going to need adjustability to get them tweaked into my OCD level of perfection. I am trying to decide, long term, do you think it would be better to program each part with its own work coordinate, or use the same work coordinate(fixture)? I lose some flexibility with doing 1 work coordinate, though that flexibility may not be needed.

In regards to the offsets, when I dial these parts in, I am trying to decide whether or not to use the control or offset in CAM. This job uses MOST of my tool holders, and a ridiculous amount ($$$) of tooling, so I do not ever see myself having dedicated tooling for the job. If I program the offsets in CAM, they are retained for the next run, I don't have to worry about documenting them. They will of course vary some run to run, but hopefully I can get it dialed in close to where first piece should be good?

Are you familiar with G10 and the Extended Work Offsets? Running this on your Brother machine? Do you have a Blum or Metrol Tool Setter?

G10 will write in the offsets each time you run the program. Make your adjustments on the G10 line(s) in the program. For Example:

G10 G90 L20 P1 X-5.000 Y-8.000 Z10.000;

this will set Extended Work Offset 1 (G54.1 P1) X, Y and Z. Your tool setter should repeat or you can write tool offsets in too with a modified G10 line. You can also save your offsets offline and load them back in when you re-run the job. When you go to Edit Mode, External I/O, there is a choice for Data Bank. Also can be done with Brother Comm software if you are using that.

Break it up. Use a separate offset for each operation/work position. You have close to 50 extended offsets. Life will be easier when it's time to adjust for wear, or adjust for other changes.

BROTHERFRANK said:

Are you familiar with G10 and the Extended Work Offsets? Running this on your Brother machine? Do you have a Blum or Metrol Tool Setter?

G10 will write in the offsets each time you run the program. Make your adjustments on the G10 line(s) in the program. For Example:

G10 G90 L20 P1 X-5.000 Y-8.000 Z10.000;

this will set Extended Work Offset 1 (G54.1 P1) X, Y and Z. Your tool setter should repeat or you can write tool offsets in too with a modified G10 line. You can also save your offsets offline and load them back in when you re-run the job. When you go to Edit Mode, External I/O, there is a choice for Data Bank. Also can be done with Brother Comm software if you are using that.

Click to expand...

This is what I use daily on my [G10 equipped] lathes.

I haven't taken time yet to figger it out on one of my Cinci mills, but I'm threat'nin to look it up soon!

On my Siemens mills, I will at least key in the offsets in the header of the program.


------------------------------------

Think Snow Eh!
Ox

BROTHERFRANK said:

Are you familiar with G10 and the Extended Work Offsets? Running this on your Brother machine? Do you have a Blum or Metrol Tool Setter?

G10 will write in the offsets each time you run the program. Make your adjustments on the G10 line(s) in the program. For Example:

G10 G90 L20 P1 X-5.000 Y-8.000 Z10.000;

this will set Extended Work Offset 1 (G54.1 P1) X, Y and Z. Your tool setter should repeat or you can write tool offsets in too with a modified G10 line. You can also save your offsets offline and load them back in when you re-run the job. When you go to Edit Mode, External I/O, there is a choice for Data Bank. Also can be done with Brother Comm software if you are using that.

Click to expand...

I am not familiar with G10, but it sounds like I want to be!

This is on my S1000. I have a Metrol Tool setter.

Is G10 covered in the manual with a decent explanation of how to set it up/how it works? Will take a look later today.

If the machine is macro-enabled, G10 is not needed.

Does the Brother control support G52Q work shifts? I generally favor this over G10 shifts, but I have Yasnac controls. If you only have 5 fixture offsets then I would just use G52-57. Work shifts really come into their own when you have 20+ parts on the fixture.

My level of OCD demands I use the control for tool offsets. I may set them in cam so if all is perfect then the offsets are 0 but all finishing paths use a G41.

DavidScott said:

Does the Brother control support G52Q work shifts? I generally favor this over G10 shifts, but I have Yasnac controls. If you only have 5 fixture offsets then I would just use G52-57. Work shifts really come into their own when you have 20+ parts on the fixture.

My level of OCD demands I use the control for tool offsets. I may set them in cam so if all is perfect then the offsets are 0 but all finishing paths use a G41.

Click to expand...

The G10 sets the G54 for you - in program.


--------------------

Think Snow Eh!
Ox

Ox said:

The G10 sets the G54 for you - in program.


--------------------

Think Snow Eh!
Ox

Click to expand...

I still have programs that use G10 so I am pretty familiar with it. You also have to set the coordinate system with a G92 to use it. With a G52Q it modifys the fixture offsets instead of setting them, if memory serves. I also have programs with G52Q shifts but since I haven't programmed them in a while I am not confident with my memory.

I got this from Vanbiker when I was asking about shifting the coordinate system.



Just to add another method to the mix...

When I need to shift X and/or Y coordinates to run a subroutine, I assign by system variable.

M98H100
#5202=2. (2" Y positive shift)
M98H100
#5201=2. (2" X positive shift)
M98H100

After running subs and at the beginning of the program I call

#5201=0
#5202=0
#5203=0

to cancel the shifts.

DavidScott said:

Does the Brother control support G52Q work shifts?

Click to expand...

Yes, it does. I use this on a repeat program I run. I put G52 Y-0.25 to tweak fixture location and the start, M30 at the end cancels it out.

DavidScott said:

.......

I got this from Vanbiker when I was asking about shifting the coordinate system.



Just to add another method to the mix...

When I need to shift X and/or Y coordinates to run a subroutine, I assign by system variable.

M98H100
#5202=2. (2" Y positive shift)
M98H100
#5201=2. (2" X positive shift)
M98H100

After running subs and at the beginning of the program I call

#5201=0
#5202=0
#5203=0

to cancel the shifts.

Click to expand...

Keep in mind that this shifts all fixture offsets(G54-G59).

I use direct assignment of fixture offsets by system variable for the repeat jobs I have that set up at a permanent fixed point on the machine. I just write them into the first lines of the program.

%
O1234
#5221=-2.3456 (Sets G54 X to -2.3456)
#5222=-3.4567 (Sets G54 Y to -3.4567)
#5223=1.2345 (Sets G54 X to 1.2345)
N1 G90 G54
Rest of program......

This method is only valid if your machine is spec'd with Macro option.

Fal Grunt said:

I am not familiar with G10, but it sounds like I want to be!

This is on my S1000. I have a Metrol Tool setter.

Is G10 covered in the manual with a decent explanation of how to set it up/how it works? Will take a look later today.

Click to expand...

It's in the manual but here's my 'Cliff Notes'. Have a separate G10 line for each offset in your program. The G90 is important because if the machine is in Incremental mode, the G10 will just add to what is in the offset. The 'L' word tells the G10 what to write to. L2 is Standard coordinates, L20 is Extended. The 'P' designates which offset. Examples: L2 P1 is G54, L2 P2 is G55, L2 P3 is G56... L20 P1 is Extended offset 1, L20 P2 is Extended #2 .... You can test out by typing in the example in my previous post into MDI and pressing start. You will see that those #s are written into Extended offset 1.

I download an offset file to my pc with the program file and keep the tools in a rack for that job. When I put it bacl I upload the program file then the offset file to the machine, bolt in the fixture, load the tools and start making parts.

Sorry, somehow I put this in the wrong thread

We have fixture subplates in our Speedios that allow various fixture plates to be accurately located each time the fixture plate is swapped out and we thusly use G10 near the beginning of all those programs. It’s still amazing to me how the first parts are virtually always right on. I still have my fingys on the rapid and feed override knobs at first but at least my heart rate is down to the low 100’s nowadays for that first cycle! Haha!

Ok, fame suit properly zipped up .....

So why again do you guys put the Workoffset call INTO the PART program?

I can understand Kustomizer's method if he has a fixture plate that doesn't move. Load part program and load Offsets, hit Green.
I can understand having a part program and a probing program. Probing runs once and loads the fixture offsets. Then only part program runs for the rest of the job.
I can understand having a probing program INSIDE the part program for complex parts. Probing program runs first, measures part and locations, shifts workoffset as needed, then part program runs.

I CANNOT understand why G10 should be in the part program? If you set the workoffset once, then why on earth re-set it every friggin' time the program runs?
Why is it better to mess with the part program to dial in a fixture offset, when you can just do it on the offset page?
Yes, if your machine has only a very limited number of workoffsets ... that is your only option, otherwise I just don't get it...

If your fixture base moves all over (vice comes off and on frequently) this may not be much help, but if you have tombstones and fixtures that are always the same place (or in the case of a lathe that X and collet/chuck face are constants) then when you pull up the program - and you hit go - all offsets are loaded. There is no forgetting or fat-fingering going to happen.

Can you really notice the time that it takes the control to scan 5 lines of code?


--------------------

Think Snow Eh!
Ox

SeymourDumore said:

........So why again do you guys put the Workoffset call INTO the PART program?.....

Click to expand...

I certainly do not do that if the fixture offset may be different from one run to the next. If the situation suits keeping the fixture offsets in the program I do it.

On jobs that do move, I still save an offset file as my vises are keyed to the table making "Y" within a thou or so and the X I save the distance from the edge of the table with a sharpie on the vise or fixture and repeat within a few of thou on replacement. Saves tools and offset files always puts me in the "good" part on the first cycle and spot on in the second cycle saving hours each time I put it back in, diameter offfsets are nice and come with the offfset file when saved.

I will try to remember to share pics of my favorite fisture in the am, at one time I had 300+ jobs running with 10 min setups on this machine.

Ox said:

If your fixture base moves all over (vice comes off and on frequently) this may not be much help, but if you have tombstones and fixtures that are always the same place (or in the case of a lathe that X and collet/chuck face are constants) then when you pull up the program - and you hit go - all offsets are loaded. There is no forgetting or fat-fingering going to happen.

Can you really notice the time that it takes the control to scan 5 lines of code?


--------------------

Think Snow Eh!
Ox

Click to expand...

Ox, I get that!
But pre-loading or probe entering the workoffsets offsets once takes care of all that and does the same thing!

What I don't understand is why dick with the part program, when the offsets are readily accessible?