[bookwurm99]

what is the real world use of G10. why would anybody use it?

[automizer]

at the shop im at we use the G10 code on a few programs. This machine has 3 vises that never move and some standard fixtureing that go in and out the same way and with 12 work zeros its nice to have the the X, Y, & Z values to be pre set. As the fixtures are always in the same place this cut set-up time from an hour to 15mins

[codyst]

It comes in handy when using a 360 degree 4th axis. It's not possible to set up offset values for every position of the table. My X and Y axis are always set off of the center line of the table, so I change the values in my work offsets as the table turns.
I also used it on a fixture that used a big slab mill to mill the back side of a part. Whenever that tool was in the spindle and was in the cutting position I would tighten up the software overtavel limits so that it couldn't be jogged into the fixture, and so that it couldn't be ran into the fixture if someone made an incorrect offset.

[psychomill]

As the other guys said.......

The most common usage of G10s are for workoffset setting. Allows the use of multiple/dedicated fixtures to repeat over and over. Very common for cell manufacturing. Allows you to set and re-set offsets 100s of times while only using a few offset coordinate sets. I also use it on stand alone machines as well. I use dedicated fixtures that mount to a grid plate (subplate) on the machine. The location of the vises or fixture plates repeat to within tenths. This allows me to use G10 offsetting in the program for repeat parts. Couple that with the use of a tool presetter, set up time is slashed considerably since we don't have to pick up any offsets for repeat work.

Other common usages: writing/updating tool offsets, writing/updating parameters, writing/updating tool data ..... and many other things.

[codyst]

Here is a picture of the part I was talking about that I tightened up the software over travels so the cutter wouldn't hit the fixture. It was held in the fixture close to the same way it's shown in the picture. The red line points out the surface that was being cut.

[ghyman]

For the past ten (ish) years, I have been running a wire brush in a live toolholder for deburring of parts in several flavors of swiss machines.
The use of the G10 allows me to bump the offset in .0002" per piece to compensate for brush wear, and by adding a check at the end of the program, I have the machine alarm out with a "change the brush" message when the offset has changed more than a preset amount.

I also did something similar on a lathe; running a finish pass on post- heat treated L605, with a CBN insert; I found that the tool wear was very consistent, very linear. I did a G10 offset bump of .0001" every three pieces.

In both cases, the jobs were run with minimal intervention by the operators... I believe the G10 is one of the handiest tools available!

[Geof]

...I also did something similar on a lathe; running a finish pass on post- heat treated L605, with a CBN insert; I found that the tool wear was very consistent, very linear. I did a G10 offset bump of .0001" every three pieces.

In both cases, the jobs were run with minimal intervention by the operators... I believe the G10 is one of the handiest tools available!

Just as a comment this would also be possible with G52 and some of the G10 applications described in the other posts can also be done with G52. For instance physchomill's multiple part offsets can be done using a single Work Offset and multiple child offsets from G52. The two taken together are extremely versatile and useful.

[ParkerMillguy]

I've used a G10 for all of these applications as well. My very first use of it was a parts counter. G10 G91 P100 R.0001

[spoiledbrat]

I may be missing something here.

Right now, using Mach 3 , I use G54, 55, etc for doing offsets. Are you suggesting that I am not limited to 6 offset tables, and that using G10, I could have infinite offsets available?

[Geof]

I may be missing something here.

Right now, using Mach 3 , I use G54, 55, etc for doing offsets. Are you suggesting that I am not limited to 6 offset tables, and that using G10, I could have infinite offsets available?

Well, sort of, yes. You can read different values into G54, 55 etc. Or as I mentioned you may be able to use G52 (if Mach 3 recognises it, I do not know).

You do have to be careful because when you do this if the program stops part way through you might not know what your offset values are. You have to be sure that at the start you set everything to the starting conditions.

Mind you infinite is a big number; your program may be a bit long .

[cnc-king]

I may be missing something here.

Right now, using Mach 3 , I use G54, 55, etc for doing offsets. Are you suggesting that I am not limited to 6 offset tables, and that using G10, I could have infinite offsets available?

you are limited to G54 thrui G59 unless your machine has the extended offset option. G10 will only allow you to modify your offsets thru your program either incrementaly or absolute

[dertsap]

Just as a comment this would also be possible with G52 and some of the G10 applications described in the other posts can also be done with G52. For instance physchomill's multiple part offsets can be done using a single Work Offset and multiple child offsets from G52. The two taken together are extremely versatile and useful.

g52 is a great little tool especially on multiple part fixturing , sub programs and g52 shifts keep it much more simple the programs are much smaller and easier for doing edits , and if the sub works on the first part it will work the same on the next provided the g52 shift is right
and as geof said are great together ,on a cell system g10 and g 52 are deadly

[HillBilly]

Camsoft really deviated from the standard on this one (G10). They use it to apply accel and decel to a feed move.

Darek

[theemudracer]

[QUOTE=ghyman;254200]For the past ten (ish) years, I have been running a wire brush in a live toolholder for deburring of parts in several flavors of swiss machines.
The use of the G10 allows me to bump the offset in .0002" per piece to compensate for brush wear, and by adding a check at the end of the program, I have the machine alarm out with a "change the brush" message when the offset has changed more than a preset amount.]

Im interested in how you program the check at the end of the prg??

I run a 18-i tb Lathe and use tool life in minutes. When a tool expires in time it finishes the part but stops at the M99 at the end of the prg. with no alarm.
It just stops with no message.

I would like to put check of some sort in there so it will alarm out if a tools time expires.

Can you help me??

thanks Jon

[adamant]

Wrote a program this week for a lathe.

Had to drill a hole all the way through a 4 in piece of plastic and then turn it and put another hole in it.

First hole drilled with material in chuck Z clearance to chuck was 1.5"

G10p0Z-4.0

brought tail stock forward, turned part with 5.5" to chuck.

drill bigger hole at the Z5.5 offset then cut it off.

At the start of the program G10P0Z0 so I did not have to check the offset all the time.


Worked great.

3 minut cycle time.

[5077phil]

I may be missing something here.

Right now, using Mach 3 , I use G54, 55, etc for doing offsets. Are you suggesting that I am not limited to 6 offset tables, and that using G10, I could have infinite offsets available?

yes, use it in the program head for work shift all on G54, set up your work holding to go back up in the same place (I use dowled chick vices), then you will have as many workshifts as you will programs, ie save program, break down, load program, put up jaws, job done

[HillBilly]

I may be missing something here.

Right now, using Mach 3 , I use G54, 55, etc for doing offsets. Are you suggesting that I am not limited to 6 offset tables, and that using G10, I could have infinite offsets available?

With Mach3 you have access to 255 work offsets. Here is a snip from the manual.

Darek

[sa.snyder]

but in a g10 situation, you must know the exact measurement from one part to the other. where as, if you use g54-g59. you can manually locate every part pretty easy. but if your running out of offsets, i can see this being good use

[Mitsui Seiki]

but in a g10 situation, you must know the exact measurement from one part to the other. where as, if you use g54-g59. you can manually locate every part pretty easy. but if your running out of offsets, i can see this being good use

You can manually locate parts just as well with G10.The only difference is that you put your values in the program instead of in the work offset page.The good thing about G10 is that you don't have to locate the part every time you run it.Let's say you run a part (1)for a week and then you do another set up for a different part.The next time you run "part1" you don't have to locate g54 g55... Just mount your fixture ,tools and load your program and you're ready to go.In order to do this you must have a fixed location for the fixture.

[sa.snyder]

o.k... i see the "big picture" now