[ios1000]

We just bought a Toyoda milling machine with a Fanuc 18i controller and I feel there should be an easier way of setting the tool length offsets. At present, we are calling up tool 1, manually inserting the tool, bring it down to work piece and set off, input number into offset, then minus the gage block, calling up tool 2 and repeating. All this while going by all the safety door switches which we have bypassed, so we need to put the safety switch "in" when we call up tools and jog machine around, but pull the switch "out" when we want to put tool in spindle manually. So you can understand that setting 10 tools can be a real pain in the neck. So my dumb question... is there a built in tool setting cycle that you can tell controller you are setting 10 tools and your gage block is 1.00" and then just cycle through it? (we have a few Fadals and that is how their tool setting cycle works). Any help will be very much appreciated. I know we are only scratching the surface what this controller can do, but we are learning the hard way. Naturally trying to call anyone for support is waste of time, 100% of the time you get voice mail and 80% of the time they never call you back. So looking for the experts here to help me out.
Thanks for all you help

[glovebox20]

I work at a shop with 3 mills with Fanuc OM controller's and fight the some of the problems you desribe.

For changeing the tools, I made a custom Tool Change program (I named it O1234) that starts at tool 1 and stops with a M0, then changes to tool 2 and stops with a M0 and so fourth. I also included "N" numbers so I can quickly search for a tools. For example, If Tool 3 is in the spindle and want tool 5, I go to Edit and Call up Program O1234 and search for "N5", filp switch to auto and run program. When program stops, filp switch to handle and I can take tool in and out. Your machine may be differnt though. When I done putting tool in and touch it off, I can go back to Auto and call up the next tool.

We do a lot of vise work in my shop, and I like to touch All my tools off at the bottom of the vise and change the Z offset according to the hight of the part. to do this, I use the Shift Cordiant offset (Z), the one before G54 (this works for the OM controller's) I use a 1-2-3 block and a 1/2 dowel pin. Before changing tools, I enter 2.5" in the Shift Cordiant Offset, and call up my tool. This updates the cordiant system. When I touch the tool off, I enter that number in the offset. when I'm ready to run the program, I add my parrell hight and my part hight together and enter that number in the Shift Cordiant offset (Z) and run program. So if my parrell is 1" and my part is .875", My Z offset would be 1.875" to get to the top of the part. I hope this makes sense to you.

As far as I know Fanuc dose not have have and custom Tool change like the fadals but maybe the 18i is different. One possiable option though is use a hight setter to measure the tools and use positive tool lenght offsets instead. This way you would only have to touch one tool off the part to fine your Z offset.

[psychomill]

As Glovebox described, you'll have to write it by way of longhand or macro. The better ways of doing this though is to either have a tool probe added to the machine or go buy an external presetter. Then, like he says, you only need to touch off one tool.

[dpuch]

A much better solution is to measure your tools oufline... In a tool presetter.
This can be a dedicated "machine" and expensive, or as simple as a precision tapered pocket and a heigth gage.

example of a mscdirect.com low end complete solution. I can't find an example of a plain tapered pocket designed for tool presetting (top edge at the gage line of the tool)

A low end alternative is to do a rough measurement from the top of the flange. I'm guesing this is either CAT40 or CAT50... The top of the flange is 0.75 from the gage line. The tolerance/accuracy will depend on your tools though.

If your offline measurements are not accurate enough or you just want to stick with measuring in the machine, with macro B you can write a macro to run thru your tools and measure them. I would suggest using a macro variable used as the location of your touch off block. Call up the tool and position it automatically as close as is safe and pause. Jog and touch off. When you restart have the macro compare the curent position to the known block position and write the offset to the control. Be careful if you have the length offset active. Make sure it does not move when you change the offset, or just do all this without activation G43.

Example of a zero move line to activate G43 for referance (We have a Toyoda 16i):
G90 G0 G43 G54 Z[28.53-[#[2000+#4120]+#[2200+#4120]]] H#4120
Z28.53 being the tool change Z This is probably better as a G91 move... I just never changed and tested it.

Unproven code to do what I suggested above. If you have broken tool detection, you could try to use the skip signal to sense the tool lenght but not all tools materials are conductive!
O8001 (TOOL TOUCHOFF)
#500=7.0 (block Z position G54 system)
#1=0
N0010
#1=#1+1
T#1
M6 ( note my M6 macro moves to tool change position and activates G43 tool length! )
G0 G54 X4.0 Y20.0 Z18.0 B0
G1 Z#500 F100.0 (if your not starting with an offset that is close, make this Z14.0 or some safe z clear position)
M0 (switch to manual and finalize tool touch off)
M20
#[2000+#4120]=#5043-#500+#[2000+#4120] (check this math and output!)
#[2200+#4120]=0 (zero length wear)
(possibly zero radius and radius wear too for safty)
M20
IF [#1LT60] GOTO 10 (loop thru 60 tools)
M30


Also ask for an applications engineer at toyoda. They have macros and subs, or may help you write stuff. You should have also gotten PDF manuals, both Toyoda machine specific and general Fanuc manuals. Look in the 63014en.pdf fanuc (16i/18i control operator) manual for control usage and programming, including macro programming.

Dale

[ios1000]

Thanks to everyone for getting back to me. The best solution I believe is to get a presetter. I was convinced there was an easier way but just didn't know it. We have an old Mori Seiki MV65 with a Yasnac controller that has a "Write & Retract" feature on its control and figured the Fanuc had to have the same kind of thing because the Mori is about 25 years old. Not a big deal, for now we'll just keep going the way we have been going. I do like Glovebox idea of writing a small program to cycle through the tools, (i'm a programmer....why didn't I think of that! lol). The macro idea is over my head, I do understand that macros can make your life alot easier as a programmer and operator but I just never wrote one on my own and would have no idea how to use them if I did. But thank you anyways because I know that is how someone that did know how, would solve this problem. Thanks again everyone, I don't feel so bad now, not as dumb question as I thought. Keep the chips fly'n

[Dan Fritz]

If you're investing in a tool presetter, then here's a way to interface that presetter to the control using tricky DNC software and a barcode reader.

Presetters are nice for getting the tooling information, but getting that information into the CNC control can still be a bit of a problem. This system lets you use the presetter to put tooling info into a database, then the DNC system pulls the data from that database using a barcoded tooling ID tag. It works with lathes and mills. For info go to:

http://www.sub-soft.com/tooling.htm