The best way to use "Fixture Offsets" In a CNC88?

[donl517]

We used work offsets everyday where I used to work. Several of the tools in the machine were common in every machine. Tool 1 was always set to a length of 0.00". We then used tool 1 to find the top of the part and set Z0 for whatever work coordinate we wanted to use. This was the first real CNC production shop I had worked in. Every where else I ever worked were Mould and Fixture shops.

Could someone give a step by step detailed walkthrough of how to go about setting up a Fadal CNC88 in a similar manner. I would like to leave certain tools in the machine always ready to run and use tool 1 to find the top of the part.

Thanks,
Don

[DareBee]

My method is not exactly what you have asked but is close.

I set all tool tips to 0.0 on the table.
You then measure or calculate the height to the top (or bottom) of your workpiece from the table.

Eg my 4th axis is 6.5 to center
my vise is 2.875 to the base + parallel + Mat thickness.
Face of 3 jaw chuck 3.937

My 4th axis is G58
Vise is G54 (axis is XY 0)
3 jaw is g55 (back jaw and work stop = 0)

Sometimes I need to pick up 1 edge for my fixture offset but frequently I need to pick up nothing.

I do not use Z offsets for the fixture. Simply because I don't know how it will work, I have never had time to piss around figuring it out (if it is even doable?) and what I do works real good anyway.

I do most of my programming in CAM and offset the regions or model above Z zero to correspond with the fixture height on the machine.

Eg If the top of my material is 5" above table and I am cutting a 1" deep slot my tool will be programmed at H(tool number)Z4.0

IF I am required to pick up or remachine a precision component I will still do a custom setup (indicate the part itself and set tools to the part itself) to ensure that my setup is the best it can be.

[mad mark]

Everyone I have always taught, I had to break old habits of setting tools to the top of a part.

In rapid prototype and production work I use common (T1-T11) tools set with a tool height setter off of the table, THEY STAY IN THE MACHINE, AND STAY SET!!!! Always use fixture offsets for x,y,& z. Way faster!!! When running 7-9 workstations for a single part every dimension is infinitely adjustable that way. No guessing the distance from the top of G54 to G56 etc...

As for the 4th axis, some times I'll run a work fixture offset off of centerline for turned parts etc..., but for the fixtures using the tombstones I use g54, g55, etc. I want each tool in the spindle ONCE for the entire part or parts!!!

Mark

[donl517]

Originally Posted by mad mark In rapid prototype and production work I use common (T1-T11) tools set with a tool height setter off of the table, THEY STAY IN THE MACHINE, AND STAY SET!!!! Always use fixture offsets for x,y,& z. Way faster!!! When running 7-9 workstations for a single part every dimension is infinitely adjustable that way. No guessing the distance from the top of G54 to G56 etc... Mark

Mark,

It sounds like you are describing exactly what I want to do. Can you give a step by step of setting up the tooling and offsets to work this way. One problem I have already run into when setting the fixture offsets the machine wants to move to X0, Y0, Z0. It looks like a recipe for disaster. Does it really make a difference as far as fixture offsets are concerned if I am running Format 1 or 2?

Thanks,
Don

[widgits]

First thing I have to ask if your using format 1 or 2
format 1 is fadals specific programming setup using E1-E99
format 2 is Fanuc compatible using G54-59 fixture offsets
So what would you rather have 99 or 6 base fixture offsets?
To check this at "ENTER NEXT COMMAND" command prompt
punch in SETP (set parameters) enter
From here you can change which format the control runs in

After 20+ years of running Fadals I have just a couple of things to say
about setting the tools and fixture offsets
KEEP IT SIMPLE!!!
I "ALWAYS" set the tool length offsets to the top Z0 of the part
ALWAYS!!!, If you do this with a tool height block or off the table
and then set a Z value into the fixture offsets this just confuses
the next guy
This also ensures that the programmed values equal the part dimensions
Unless you like back calculating numbers
The only time I use a Z value fixture offsets is when I have multiple
parts and this value is the difference in height between E1 and E2
either plus or minus
So this means that fixture offset E1 has no Z value
To find this height for E2-E3-E4 etc
just write down the tool length offset for T1
Jog T1 over and touch it to the top of the part at E2
subtract this new E2 value from the tool length offset value of T1
you wrote down earlier
and enter this difference into the control at fixture #2

The machine will now change the tool heights for the next fixture offset
If you break a tool just jog back to the first surface you set all the tools
lengths at in the initial setup E1 and punch in SL,1 or SL,2 etc. and enter

Pretty simple and easy control to learn
But if you get into the fixture offset utilities
Just wait till someone sees you locate a round part with an edge finder
to find a center
Yes, you just read this correctly
Locate the center of a round part with an edge finder
It works very well and accuratly
I didn't believe it myself at first, Then I checked it with an indicator
I was off only about .0005" TIR

Hope this helps
Widgits

[mad mark]

I've always used format 2............

moved to xo yo zo?? machine zero's???

try G0 G90 G54 X0 Y0, don't call up Z0 you have to have the tool height offset in there for whatever tool is in the spindle.....

t1m6
g0 g90 g54 x0 y0 z5.0 h1......
t2m6
g0 g90 g54 x0y0 z5.0 h2......
this will go to E1 or g54 and 5" above the part with that tool only. This is why when you use multiple wfo's you don't set the tools to the top of one part, SET THEM TO A COMMON HEIGHT FROM THE TABLE!

[donl517]

Originally Posted by mad mark moved to xo yo zo?? machine zero's???

Not the machine 0's but the Offset 0's. I did not have a Z height called only X & y but it went to Z 0 anyway. The next line had my H1 Z0.1 tool height call, so then it moved 0.1 above the part. Luckily I had called the length of the tool 0 and had used it to pick up the top of the part. Apparently that is not going to work.

1. So set the tools to a common plane.
2. How do I then find the top of part for the fixture offset? Can I use tool 1?

Sorry if I'm a little dense on this but it is not working at all how I was used to it.

Don

[donl517]

Originally Posted by widgits KEEP IT SIMPLE!!! I "ALWAYS" set the tool length offsets to the top Z0 of the part ALWAYS!!!, If you do this with a tool height block or off the table and then set a Z value into the fixture offsets this just confuses the next guy

Hi Widgits,

Yeah I ran a Fadal for about 6 years back in the 90's, and that is how I always did it too. However, having worked in a production environment I found I do like not having to touch every tool every setup. It was great to grab tool 1 and touch the top of the part and the first 10 tools were set just like that. For that reason tool 1 always had a length of 0, all the other tools were comped from that. As far as the "next guy", that's me too! I'm confused most of the time anyway so I don't think this procedure can hurt to much.

Thanks for the feedback,
Don

[mad mark]

most lean shops will tell you that things need to be standardized, if the next guy is confused or wants to run a job differently, train him on the standard. Minimizing set-ups on prototype and production is the name of the game, and not having to reset tools every job is step #1!!! Have a standard tool list at each machine ie.....t1=3" face mill t2=3/4" rough end mill t3=1/2" rough end mill etc......those tools are set and stay put every job.....in order to do this you have to set the tools to a place other than the top of the part!!!! Fadal format 2 recognizes E values so have your post out put e1, e2, e3, etc....

Your fixture offset is the difference between where the tools are set and the fixture you're using. Off of the table that would be a positive value. If I had to reset tools at my old job where we had 300+ tool magazines a 1 hour set-up would have taken ten hours and I'd be looking for another job!!!

[Edster]

Just wait till someone sees you locate a round part with an edge finder to find a center Yes, you just read this correctly Locate the center of a round part with an edge finder It works very well and accuratly I didn't believe it myself at first, Then I checked it with an indicator I was off only about .0005" TIR

Could you elaborate on this a little? I'd definatly have a use for this tip. Do you need to start in the apporximate center of the circle, or will any three spots work?

I program all my tools off the table or bed of the vise, whichever I'm using. I end up putting a positive offset in the z value of the fixture offset. The problem with fadal format 1 is when you call the offset, even if you don't specify a z move the machine will try to adjust the z the ammount of the offset. This means with 2.000 in the z offset for E1, then a G0X1.Y-1.E1 the machine ends up moving the z axis up two inches. I don't know if this is true for format 2 or not. This is certainly not the case with my old Haas TM-1 or new Okuma MCV4020. To get around the problem I put the x y z move and call the Tool and work offset in the same line. I don't like this method because Fadals slow down all the axis when one axis decelerates. Does anyone know if this happens in format 2?

[Geof]

Originally Posted by DareBee ....Eg If the top of my material is 5" above table and I am cutting a 1" deep slot my tool will be programmed at H(tool number)Z4.0...

We do things very similar to Darbee with one difference: Our reference point is not at the table but at a point higher than the highest part. We do production on our own products so we know how high that is.

The reason for this is because errors get made in number entry: One possible error is punching the negative sign when the value to be entered should be positive.

If the value should be positive and a negative is entered you finish up a long way further down than you should be with probably disatrous consequences.

If the value should be negative and a positive is entered you finish up machining air which is much quieter.

[dertsap]

the best experience that i had in a production environment was to have all the tools located from the table (tool probe) , we designed the fixturing with locating pins , on the virtical we had a sub plate that all the fixtures bolted to , on the horizontal the tombstones were fitted the same , everything was set using g10 and a lot of use of g52 shifts , it was idiot proof drop the fixture on load the programs press cycle start and walk away
the use of keeping the same tools and setting up in a way that a fixture always locates in the same position is a huge time saver in the long run especially when g10 can be utilized