[Shizzlemah]

Hey folks,
What's the proper sequence to set tool and work offsets?
Do I set all my tool offsets in the E0 coord system?
Then how do I set the fixture offsets? With or without loading a tool to indicate the fixtures?

Thanks

[DareBee]

I set all my tools to Z zero on the table and then I set the part Z offset in my CAM software when I program (My parts are VERY seldom over programmed at Z0).
I have multi fixtures on my table most of the time (vise, 3-jaw chuck, 4th axis,etc) and each one is datumed (X,Y) with it's own offset designation (G53, G54, G55...). So I program my part to fit the previously setup fixture, and then the machine setup is often nothing other than loading material and DNCing the program.

[Shizzlemah]

Okay that helps a bit, a couple of qeustions though.

If you have a 3" block in a vice that's 2" tall, do you tell the cam SW that your block is 5" tall?

What happens when you go to a 4" tall cylinder in the 3-jaw that is also 4" tall by itself?

Do you have fixture offsets that adress that Z difference between fixtures?

Thanks

[Shizzlemah]

Well here is what I came up with to define Z=0 at the surface of the workpiece. Let me know if this is screwy or could be better.

1) Set all tools for length using the table as Z=0
2) Find X0 Y0 of each fixture and set those fixture offsets.
3) Go to E0, load a tool and apply height offset.
4) touch off that tool on each fixture to measure Z height, record DRO reading
5) edit fixture offset table adding Z heights as measured above.


Good, bad, indifferent??

[screensnot]

Well here is what I came up with to define Z=0 at the surface of the workpiece. Let me know if this is screwy or could be better.

1) Set all tools for length using the table as Z=0
2) Find X0 Y0 of each fixture and set those fixture offsets.
3) Go to E0, load a tool and apply height offset.
4) touch off that tool on each fixture to measure Z height, record DRO reading
5) edit fixture offset table adding Z heights as measured above.


Good, bad, indifferent??

I think that is a good way to do it. Not the way I do it, but you have to do what suits you best.

Advantages to your way are many:

> Easy to reset a tool
> Easy to go from fixture offset to offset (no tool offset adjustment is needed)
> Makes it easy to have up to 99 (I think) tools setup with their own offsets stored in machine
> Probably more resons that I can't think of at the moment (probably cause I don't do it this way)

The one disadvantage that I can think of is the reason I don't use that method:

> You forget to call a fixture offset in your program, and move the tool to Z0 (or god forbid a negative number), and your are going to have a crash.

---

The way I do it suits me for my one offs, and low volume, different part everyday type of work.

I don't use fixture offsets (very often). I set the tools in E0 to wherever is a convenient Z0 for me, on whatever part I am currently working on.

When I switch to the next part, I am usually breaking the tools down, and changing to different ones anyway. I haven't got enough holders to keep them setup.

When I can keep some of the same tools from job to job, I just mass modify the tool offsets. Then I change or add whatever new tools I need and just set the new ones.

Now when I write my programs I don't have to worry about calling a fixture offset, just the tool offset.

The rare occasion that I do have a couple of fixtures, or maybe a 3-jaw chuck setup, I may use fixture offsets to remember the position of X0,Y0 for them. But when I actually switch over to use them, I reset X,Y so that I am always running in E0.

---

There was a guy that came into out shop that liked to use a fixture offset that set the spindle face to Z0 so that all his tool offsets are positive numbers and are equal to the actual tool length (with holder). I think that is probably the best method if you are going to be doing tool pre-setting (with an off-line setter).

You can easily pre-set with your method also. You just need to find that certain number that will need to be subtracted from the actual tool length, in order to get the proper tool offset.

Even if you don't pre-set, it would be kind of cool to be able to just look at a tool and estimate if the offset is in the ballpark. Or slap a scale up against it when something doesn't look right.

We do use this method on some of our machines, but not the Fadals.

[DareBee]

Well written.
I dont use an offline setter so it is quickest for me to set to the table.
Other guys I know that only use a couple of tools for each job, set each tool individually on there parts (mouldmakers). I tend to do a lot of drilling and tapping and it is not uncommon for me to use all 21 slots in my ATC. Z zero on the table saves a lot of setup if I am reusing same tools for next job.
Also I NEVER set Z offsets in my machine control (this may be stupid but it is what I do), I always program my part in CAM with the Z level where it will be fixtured. EG my Kurt vise is 2.875 my parallel is 1" and my raw stock is .75 therefore in my CAM I will set the top of my stock (in space) at Z=4.625 while I am programming. So if I am taking a .100 cut and my Z0 (tool offset to the table) happens to be -19.562 then my cutter will pass at -15.037
Clear as mud...huh
I also like this option of setup (for me anyway) because I sometimes do simultaneous consecutive secondary OPs ( to save tool change times) in a second vise (just paste 2 programs together) and the z setting is relevant without making any changes at the machine control.

[ghyman]

Just my 2 cents worth, but I like setting all of my tools to a common set plane (the table, or a gage block, or something consistant all the time), and then establishing Z0 for each job using its own E word (or G55/56/57/whatever). This gives me the ability to always have a good idea what the program is doing, without having to subtract part height or vise height or anything else.

But I will NEVER agree to setting each tool differently... Z0=the top of part A for tools 1-5, Z0=the center of the hole in part B for tools 6 and 14, Z0=the bottom of the T-slot for part C with tools 7,8,and 19... etc.

Common tool plane referencing is the safest and most sensible (in my book) way to set up a machine. As far as where to put Z0, my preference has always been to use a fixture offset for each new part. That may not be the BEST way, but as I said... just my 2 cents worth!

[carbidecraters]

We generally set-up about 9 jopbs per day in our machines and we NEVER set a Z tool height off the table...to my thinking you are asking for longer programming times. We use a .10005 block and msc scraps of paper to sweep under the cutter in .0001 jog mode and then set the height to that Z plus -.0025 (thickness of the paper). Setting tool height is a very basic fundamental of cnc machining and should be one of the first things to learn

We also set each tool independently