Fadal Format 1 Programming

Hi Guys,

I'm working on a new post processor for an older (1991-92) Fadal 4020 5 axis VMC for some new CAM software. I was hoping that somebody could post a couple of snippets of code or short sample programs for me to examine and reference. I am new to Fadal but old to CNC and I would have to say the Fadal behaves a little differently that many other machines I've worked with in the past.

We are working in format 1. Right now I'm only concerned with getting a streamlined post for three axis work.

So here is what I am looking for specifically,
Preparatory start and safety lines
Tool changes
End of Program
Fixture offset calls
A/B Head rotations.

Thanks in advance

Tom Lipton

%
O135 (part xyz 'Letter O followed by program number' 'Parenthesis (is for comments and will show program name at the control'

T7 M6 'tool number, M6 for toolchange'

G0 G8 G90 X0 Y0 S6500 M3 E1 'Rapid (duh), G8 turns off dwell at position between moves. Smoother motion but *may* loose some contour accuracy, M3 spindle CW, E1 is work coordinate call'

Z1.2 H7 M8 'H for tool comp, M8 for flood coolant'
...

G0 G49 G90 Z0 'G49 cancels tool comp, G90 ensures absolute coordinates to return head to toolchange height'
T8 M6
...

M5 M9 'turn off spindle and coolant'
G0 G49 G90 Z0
X0 Y0 E0 'cancel work coordinate to return to 'home' position, which could be table forward
M2
%


Arc centers are relative coordinates, FWIW.

I'm pretty much clueless for A and B axis.

Tlipton, my 2 cents since you didn't ask.

Ditch Format 1, its acting funny because of Format 1. Format 1 was designed for finger cam, so it does a lot of things automatically, not all of which are desirable.

The good things about Format 2, Fanuc compatible, though the rigid tapping cycle is different, and possible a few others. You can still use all the Fadal features, like the E offsets(or your G53 G54s....). You don't need a G43 when calling a height offset, but its perfectly happy taking it. You can use G28G90blah blah, but you don't have to. You can still use all the Fadal specific canned cycles, pocketing, engravng, serializing.

I've accidentally posted Fanucese and sent it off to the Fadal without even looking at the code and perfect parts, no crashes.

Why try and reinvent the wheel. A couple little tweaks on a Fanuc post and your done.

WesG's sample will work Format 1 or Format 2. The manuals are available online for free also so that you can see the differences between Format 1 and Format 2 and its written reasonable well as far as the codes go. CNCpros is one place where they can be had, good place for parts and tech support also.

Thanks for answering Wes and Bob.

I have had the same thought myself. There are some legacy problems that I may have to work around if I switch over but what the heck I'm the boss so I can do anything I want. I was wondering about those G8 calls in some of the programs. I attributed the clunky movements to the vintage of the machine not path smoothing codes.

What are the ramifications of switching back and forth between Format 1 and 2? I have not checked to see how this actually occurs. Is it just a call in the header of the program or are we talking parameter changes and things like that?

Some of the wierd things that bother me are unexpected motion moves when I call out a simple fixture offset or tool length. This behavior seems pretty much unique to the Fadal since all I had to do with other machines is re-arrange the order of the calls to get the machine to behave predictably (Yasnac, Okuma, Fanuc).

This is the machine I will be working with for quite a while now and I'm anxious to get my brain around it. Its actually a true 5 axis continuous machine. When they first told me it was five axis I just assumed positioning but I have seen some parts and video of the thing actually moving 5 axes at once.

Thanks for the help. I'll keep you posted on my progress or lack there of.

Regards,

Tom Lipton

tlipton said:

What are the ramifications of switching back and forth between Format 1 and 2? I have not checked to see how this actually occurs.

Click to expand...

Format 1 to Format 2 is really no big deal, it is in the parameters, but its not like Fanuc parameters, its easy and simple and in english and it will walk you through it. From the "enter next command line" 'setp'. Follow the directions, power down and power up.

Some of the wierd things that bother me are unexpected motion moves when I call out a simple fixture offset or tool length. This behavior seems pretty much unique to the Fadal since all I had to do with other machines is re-arrange the order of the calls to get the machine to behave predictably (Yasnac, Okuma, Fanuc).

Click to expand...

Thats format 1, that will all go away in Format 2.

This is the machine I will be working with for quite a while now and I'm anxious to get my brain around it. Its actually a true 5 axis continuous machine. When they first told me it was five axis I just assumed positioning but I have seen some parts and video of the thing actually moving 5 axes at once.

Click to expand...

One word of caution with the true multi axis movements, you will be feed limited, its a pretty handy and friendly control, but its not fast. I've never had the fun of 5 axis, but I've done 4 axis continuous and it would only move so fast.

Once you get used to the control I think you'll like it, its pretty simple, quite a bit different from a Fanuc, or anything else for that matter, but it sure is friendly, pretty much tells you what to do.