[peterson76]

Hey guys,

I have been working with 850sx's on my Cincinnati machines for years now and I am very comfortable and possibly a bit spoiled. Especially when it comes to tool offsets. With the 850, I set tool lengths then g92 x0 y0 z0 at my stock and everything just goes fine after that, I can set 10+ tools, set x0 y0 z0 and be cutting in 5 minutes.

I also have a lathe with a Fanuc 3T, same thing, G92 and its ready to go (assuming tool offsets are done).

I picked up a Hitachi Seiki vs50 with Fanuc 16i control at an auction. I have wanted a Fanuc for awhile, if for no other reason, just to learn a new controller. Well, this machine has been here for over a week and I still have yet to set tool lengths on 2 tools and get them to both say Z0 at the face of my stock. "G92 Z0.0" does not change Z to 0.0, sometimes it does, sometimes it does not, sometimes it changes X and/or Y. If I use G43 or G44 then I get a Z over-travel in either direction. I have tried setting G54 at the work surface, Z does not equal 0.0, G92 does not do it, G52 does not do it. I have gotten so frustrated that it is just sitting there turned off while I use the Cincinnati mills.

I know this is asking alot, but can someone please post a step-by-step to set more than one tool length and zero Z at the surface of a stock for the tools?

Assuming the following: no tool lengths set, no work offsets set, no ref gauge set. Just a machine with tools sitting in it.

I feel like an idiot, any help would be appreciated.

Eric

[CNC_Monkey]

We use the "positive length offsets" method for setting up our machines.
Step 1. Measure the distance from the spindle gauge line to the top of the work table. put this value as a negative number in the work coordinate registry i.e. G54 Z-10.
Step 2. Measure the tool length from the gauge line and put the value as a positive number in the tool registry corresponding to the tool number in the magazine. i.e. Tool # 1 would go into the registry in slot 1 under "Length" with a positive value of 4"
Step 3. Rinse and repeat for all the tools you intend to use.
Step 4. Measure the height of your fixture or vise , if any, and put that as a positive value in the G52 in the work coordinate registry as the Z axis shift.
When you start to run production, set the work coordinate system to G54, then program calls T1 and using G43 H1 subtracts the positive tool length value from the G54 negative Z value as well as the G52 shift resulting in the proper tool length for that tool.
We use this system because the tool length stays the same regardless for fixture height or material thickness. (we switch both frequently.) The other benefit for us is that there are no Z- moves, since the top of the fixture becomes the part Z zero reference. So our inexperienced operators can avoid making unwanted modifications to the machine...
Hope that helps.

[peterson76]

Thanks for the help monkey, it clears up alot. one question i have is regarding step 1. Where do i put the spindle when i "G54 Z-10"?

To further complicate the issue, I'll get more specific about my setup. I have a 200mm touch probe and a tool setter block.

When I try to emulate your procedure, I load the probe and touch the setter block. This puts the machine coordinate at Z-296.0mm. I enter G54 Z-496.0, to account for probe length. Then i load tool #1 and touch the setter, this measures 163mm (that is the correct tool length), this gets put into the length field of tool 1. Then i load tool 2 and repeat. The tool lengths are correct.

Then I load the probe, touch the surface of my stock, and enter the machine coordinate (+200mm for probe length) into G55 (my buddy said just use G55 so G54 can be saved for tool setting, is he correct?).

Then I load tool 1, G55, and G43 H1 (at this point the machine gets over travel +Z but the G43 is applied) When I bring tool 1 to the surface of the stock it reads Z0.0 (thats correct).

Then I load tool 2, G43 H2 (at this point the machine gets over travel +Z but the G43 is applied) When I bring tool 2 to the surface of the stock it reads Z0.0 (thats correct).

So, basically its working. But my method has got to be the ugliest possible way of doing it. How can I do this better, get rid of the over travel alarms, etc?

Thanks in advance, and thanks Monkey for the help.

[CNC_Monkey]

In Step 1. Use your touch probe in the spindle to measure the distance from machine home (the spindle as far "up" as it will go) to the work table. If you use the Position (POS) screen you will see a "Machine" set of coordinates. They should start at Z0 and as you jog down, they should become negative. When you get the distance from machine Z0 to the top of your work table, put that into G55.
I don't know why your buddy says keep G54 for setting tools, that's OK. It works fine. I would set up G55 different from G54, G56, G57, etc. to use different fixtures if you have them. For example, G54 would be my Vise. G55 would be for some fixture that I use all the time, etc.
As far as the over travel thing, do you have G91, incremental on? Between tool changes try:
G28G91Z0 (this should move the spindle to machine Z0)
G90(this sets absolute coordinates again.)
T1(select the next tool)
Hope this helps.