why does the fadal do strange moves

[Gmaan]

I started to work on a fadal 4020 at the m02 or m30 line it moves around with no aperant reason? how do I get it to just retract the z axis turn off the spindle and move the table out so I can load parts into the vise?

Format

M9
G28G91Z0M5
M30

[little bubba]

I'm guessing that you are in Format 1, at the M30 its going back home wheather you like it or not.

[Gmaan]

How do I stop it

[scadvice]

I have not used subroutines for a long time but If I recall right, M30 is signaling the "end of all subroutines" in Fadal programming as apposed to "end of program" in Fanuc programming. This means that when the Fadal control sees this, it tries to find and return to the MAIN program.
Someone correct me if I'm wrong. Replace the M30 with M02 if that is the end of the program. If it is not the end of the program, remove it. If it is a subroutine, the start of all subroutines maybe missing. ( sorry I do not have the M Code list with me to look it up) ...thus the machine confusion.
Steve

[Gmaan]

I did originaly have a m02 at the end, but tried a m30 same thing?

[scadvice]

in Fadal programming. As I said, it means the end of all subroutines. Use m02 for end of program. It sounds like you have a command in your program that may be telling the control to look for a subprogram or a variable. Other things can be a incremental move when you mean a absolute , a "E" command ( E's are the same as G54 ect.) in other words a datum shift command you do not want.
Steve

[Gmaan]

I am format 1 here is an example of my posted program from Surfcam
N1G28G91Z0M5
G0G17G40G80G90G98
M6T5
G54X0Y0M3S3500
G43Z3.H5M8
....
....
M9
G28G91Z0M5
M1
(*)
NEXT TOOL AND SO ON.
I use this format it is a good generice format that works on almost any type of machine.
I do not post sud programs when making nc code VIA my Surfcam.

[Delw]

Originally Posted by Gmaan I started to work on a fadal 4020 at the m02 or m30 line it moves around with no aperant reason? how do I get it to just retract the z axis turn off the spindle and move the table out so I can load parts into the vise? Format M9 G28G91Z0M5 M30

I think I know what your talking about,
at the end of the program M30 the the machine will make a move this way or that way. then to home.

I believe its cancleing out its "E" offset then findinh True machine position then going to the home position for the next batch of parts to run the program again.

if you want your table to come closer to the doors to make part loading easier you need to set it up in your home position screen. For example on a 40x20 or a 60x30 the table when at its machine home postition its pretty far out , on the 40x20 I would run it to +10 inches in the screen and all my E offsets are based off of that.

in the book it tells you exactly how to do it.
what happens is basically the machine goes to home then slides 10" towards the door from the machine home( where you put the machine for CS command.

If you dont have a book I can grab it off some PDF files I have and paste it


You can not do it before an m30 or m02 cause that means end of program and your machine will cancle itself out and go back home. It must be dont on the set-up page.

oh yeah you will also get a question on your screen after you do a CS command to ask you if you want to goto your programmed home position and you answer yes or no.

you E values will be based off your self set y axis thats why I always used 10" in the 40x20 machine.

I don't use that set up anymore as my 8 year daughter knows how to put it in jog and bring the machine to the 9-10 inch mark load the parts then hit the button. Plus this way she don't have to manually move the machine to its position( marks on the machine) to do a CS(cold start), when we fire the machine up on a 40x20 she cant see the y mark very well and has missed on occasion .

[mactec54]

Hi Gmaan

Try this
At the end of your X Y moves put
G0Z2.
M9
M5
G0Y5.
M30

Take out the G28G91 Line
If you are doing a tool change don't have the G0Y move or the M30

[little bubba]

Why not just go to Format 2 so that the machine just stops where it is at the end of a program? All the weird movements at the end of a program and at tool changes is why I moved to Format 2 very shortly after starting to play with Fadals.

Gmaan, format 2 is "fanuc" compatible, Format 1 is Fadals own little thing, which does make it easier to handcode. Since you are using G28s and G43s, I'm guessing that you are comfortable with standard Fanuc programming, just go to Format 2.

On the CS vs Home, I leave the home at the CS and my post brings the table to E0X0Y9.5 at the end(I like the E's over the G5x's). If I'm working on one side or the other of the table, real easy to change the X #. I do this so that I can just send her home and shut her down, fire it back up, CS, and I'm running.

[Delw]

Bubba I never ran format 2 in 18 years, would it be like the old acroloc to were you could just run you lets say a z axis move only and the x and Y would always stay at the same position even when an m30 comes into play?

I got this one job that I run once a month used to run it in the acroloc due to this, now I just run it in the manual mill cause it took longer to get into position than run the operation.

[little bubba]

Del, exactly, you could probably take that Acroloc program and throw it directly into the Fadal and it would work. Format 2 should be close to 100% Fanuc compatible while also allowing you to use some of the handy Fadal stuff.

You can use Exx or G5xx, I prefer the E's.

Or as Gmaan is using G91G28Z0, G0H0Z0 will get you the same thing.

Gmaan is using G43's you still don't need them in Format 2, just a G0H1Z.1, if G43 is there, its not going to hurt or harm anything.

The biggest difference, besides the table going where you don't want it to go is the canned cycles. I know the rigid tapping cycles from Format1 and Format2 are different, and possibly some of the other drilling cycles(its been a few years).

Format 1 was designed to limit keystrokes when handcoding on a piece of paper and typing it in.

One other thing, Format 1 automatically pulls up your D offset when applying the H offset(or does it pull it in(D&H) automatically when calling the tool??), in format 2 you have to apply the D offset, just like a Fanuc. Not a big deal and gives you the freedom to apply multiple D and H offsets to a single tool.

I'm sitting here talking about flexibility and control of what the machine is doing, and I like conversational programming, go figure??