fadal 88hs fixture & tool offsets

I can cold start the heck out of this machine, jog it about, etc...i just cannot figure out the fixture / tool length offsets.
I've tried for about 6 hours total on two different days. with every method i read about. and I've read 5 threads here and elsewhere about modes 1, 2 E1. G54 etc....

I'm in mode 2 btw,

It just wants to stuff my tool well below the part surface, or ignore my offsets completely it,s nowhere close. luckily I am starting well off to the side of the part so I haven't crashed anything.. I have to slide hold and return it each time.

My tool length method is adapted from the way I grew accustomed from my old mill, maybe it's totally wrong for this machine? here it is:

I have one "master tool/edge finder" I'm accustomed to measuring and entering all my other tools relative to it. it's about 2" from spindle face to tip so most of my tools are an inch or so longer than it. I use a height gage and a block as a presetter. My tools all have various +Z entries in the the table.

actually I've tried - and + values.

After cold starting the machine I jog to the part surface with my "T1 Master Tool" in spindle and I look at the z height and remember it, then I go to the space menu for offsets and enter the Z height (say -9.000 ish to get down to my part top in vise with master tool) in the fixture offsets #1 I'll put in Z=-9

my most recent code looks like this: (WITH MY COMMENTS ADDED HERE IN PARENTHESES)

%
N1O9191 (program #9191)
N1.5G90G54T11M6H11 (g90 =absolute csys from "cold start"? g54=doesn't this call offset #1?, t11m6= load pocket 11, h11=tool offset #11)
N2S3500M3
N3G0X0.95Y-2.2Z1 (PART IS A LITTLE OFF CENTER OF TABLE, AND RETRACT PLANE IS 1" ABOVE PART)
N4G1Z0F35 (FACE THE PART AT Z0 PLANE. (I LIED A LITTLE WHEN I INDICATED SO I WOULD CLEAN UP THE TOP SURFACE FACING IT)
N5.........(MOVES)........
N6.......(ETC..)...




please.
at witts end.



one of the previous owners files for reference
%
N1O1
N2(PROGRAM NAME - RONS CRANK 1)
N3(DATE=DD-MM-YY - 23-03-11 TIME=HH:MM - 22:00)
N100G20
N102G0G17G40G49G80G90
N103( 1/4 FLAT ENDMILL TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .25)
N104T4M6
N106G0G90G54X0Y0A0S7500M3
N108G43H4Z0.25M8
N110Z0.1
N112G1Z0F50.
N114G3G41D4X-0.0628Y-0.1515R+0.082F25.
N116X0.0628Y0.1515Z-0.04R+0.164
N118X-0.0628Y-0.1515Z-0.08R+0.164
N120X0.0628Y0.1515Z-0.12R+0.164
etc.....

I have this same machine and we always use negative offsets in z with it. I go to the UT menu (just type in UT at the enter next command output) and just touch all my tools off the top of the part with a .5" gage block. For fixture offsets use the same UT menu, it gives you options for using an edge finder to automatically calculate the dia offset. I'm in the fadal format which i think is format 1 but it shouldn't matter really. I use E's for fixture offsets. I can give you more info when i'm at work tomorrow.

okay...

Okay, for picking up tools, try this....
I use 2 methods, both amount to the same thing.
Put your mastertool on the bench.

Assuming T1 is a facemill/endmill of some sort, Take a light skim cut by jogging the cutter across the top of the stock.

manual to exit jog mode
on the enter next command line, type SL,1
this SetsLength, offset 1 to where you have the Z axis jogged.
press manual get to MDI
M6T2 <ENTER>
PRESS JOG
JOG TOOL IN Z TO (.500 BLOCK IN THIS EXAMPLE)
MANUAL KEY TO EXIT JOG MODE
ON ENTER NEXT COMMANDLINE TYPE SL,2, <ENTER> THEN SL,2,-(THICKNESS OF FEELER)
THE SL,2 SETS THE LENGTH TO THE ACTUAL JOG POSITION, THE SL,2,-.500 ADJUSTS OFFSET 2 IN THE - DIRECTION TO ACCOUNT FOR THE .500 GAGE BLOCK
MANUAL TO GET TO MDI
M6T3<ENTER> AND SO ON

You also have a tool setting mode in the UT menu.
UT, enter
1 (tool setting mode)
tool you want to start with
tool you want to end on
enter thickness of feeler
2 (jog to set length)
jog to your feeler gage
press manual once (this is important or you can kick out of the mode)
next tool should load
lather, rinse and repeat until all tools touched off.

With these 2 methods, your G54 Z OFFSET WILL START AT ZERO. This sets the part zero to where you touched off your tools.

For your fixture offsets I recommend using the menu in the UT page.
Enter next Command line
UT<enter>
2 (fixture offsets)
1 (select offset)
1 (I use format 1, so sets E1, you might need to put 54 in format 2, not 100% sure)
enter edgefinder diameter
2000 (whatever rpms you want to run, note spindle doesnt come on)
select jog to position ( will put you in jog mode, shift+spindle on to turn spindle on)
jog to X side of part, press manual once to exit jog, back to menu
3 for store position, pick X it will ask you which side the LOCATOR is on, so it knows which way to shift the comp for half the edgefinder diameter. if on the left side, pick -, right side pick +
select jog to position again, jog off part, move to y side of part, press manual to exit jog, back to menu, 3 to store position, pick Y pick +/- to indicate which side the LOCATOR is on. you are done.

If you are indicating a hole for x0y0 you use the same procedure except pick 0 for locator diameter, and no rpm, jog indicator until you have picked up the bore, select 3 for store position, pick x, pick y and it will have your current position stored.



And your code is...not right.

one of The previous owners files for reference <------TRY THIS FORMAT!!!!!!
%
N1O1
N2(PROGRAM NAME - RONS CRANK 1)
N3(DATE=DD-MM-YY - 23-03-11 TIME=HH:MM - 22:00)
N100G20
N102G0G17G40G49G80G90
N103( 1/4 FLAT ENDMILL TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .25)
N104T4M6
N106G0G90G54X0Y0A0S7500M3
N108G43H4Z0.25M8
N110Z0.1
N112G1Z0F50.
N114G3G41D4X-0.0628Y-0.1515R+0.082F25.
N116X0.0628Y0.1515Z-0.04R+0.164
N118X-0.0628Y-0.1515Z-0.08R+0.164
N120X0.0628Y0.1515Z-0.12R+0.164
etc.....

%
N1O9191 (program #9191)
N1.5G90G54T11M6H11 (g90 =absolute csys from "cold start"? g54=doesn't this call offset #1?, t11m6= load pocket 11, h11=tool offset #11)
N2S3500M3
N3G0X0.95Y-2.2Z1 (PART IS A LITTLE OFF CENTER OF TABLE, AND RETRACT PLANE IS 1" ABOVE PART)
N4G1Z0F35 (FACE THE PART AT Z0 PLANE. (I LIED A LITTLE WHEN I INDICATED SO I WOULD CLEAN UP THE TOP SURFACE FACING IT)
N5.........(MOVES)........
N6.......(ETC..)...

G90= sets absolute coordinates Positioning.
G54 = offset 1 from "home". As discussed in the other thread, this may or may not be your CS position.
M6T11=TOOL CHANGE TO T11 **note** only codes on this line should be M#T# and comment after either ( or *
H11=Tool length offset 11

in my experience on Fadals, your format should be more like this

%
O1*Program Name
M6T1*TOOL COMMENT
S6500M3
G0G90G54X0Y0A0*OBVIOUSLY WHATEVER YOUR XY SHOULD REALLY BE, A=4TH AXIS ANGLE
G43H1Z.1M8 * G43 IS OPTIONAL IN FORMAT 1
**** VARIOUS MOVES *****
G0Z.1M5M9
G49Z0* CANCEL LENGTH OFFSET, RETURN TO MACHINE Z0 <--SHOULD BE YOUR TOOL CHANGE POSITION
M1

Your program picks up the tool offset with a call out of the letter "H". The sample you provided is using "G43".

Using the format you're using, should you have a "g43" instead of the "H"?

I have seen it both ways.
I typically use the line like this

H1Z.1M8