Fadal Programmers, a bit of help?

Not a Fadal guy, but I imagine it has something to do with how the machine handles a G80 or how G28 is set in the control. Either way a G54 Z0 move can be a really bad thing, depending on where your G54 is set at. A few things to look at:

1) Sometimes decimal points matter, so try G28 Z0.0 instead.

2) Try a G53 Z0.0 in place of the G28 Z0

3) Long shot, but you can try using G55 for the program and set G54 to some higher value to see if it goes to G55 Z0 or G54 Z0. 

On second look, I think you're missing an incremental call. G28 Z0 should be G28 G91 Z0

Not a Fadal guy either but It might be that you need to call the G80 on the next line after the canned cycle or at least use a g90 or g91 before your x axis moves.

N60 Z0.3

N61 G73 R0-1.7 Z-2.06 F2.5 Q0.04

N61.5 G80

N62 G90/G91 G0 X4.365

N63 G0 X4.385

N64 M9 M19

N65 G80

N66 G28 Z0

N67 M30

G91 should solve your problem. If left in the absolute mode it will go to G54 Z0 then to machine home, which is exactly what its doing. G90/G91 behaves a bit differently with the G28. Its not a FADAL thing.

You getting what you want out of N64?

You guys are making me moist.

I've only done some simple stuff on my own. 99.9% of everything I did Mastercam figured it out. All I really did after hitting "create toolpath" was dial in feeds and speeds. Oh, and try importing shit from Apple software and find the micro loop in a line somewhere. Master Cam can find it now, but before that....schize...

Nice work, boys.

You shouldn't need the spindle orient (M19), it should do that automatically for the tool change at M6. You'll want an M5 (stop spindle), though. 

Here's a full drilling cycle from my machine (Hurco, but most of it should apply to Fadal)

Multiple M codes on a single line.

M19 before an M5 (ouch).

No reason for the M19. 

In Luxon’s program notice the M9/M5 consecutive. Put the M5 after the Z home and let the spindle sling off the coolant.

So the G81/83 only needs to be called once and will be called automatically after each subsequent block until G80?

I will will have to look at my drill cycle code. it may be the same. I just don't remember.

Correct, you just use one call for the canned cycle, then drill coordinates, then G80 to cancel

OK. I just checked and Linux CNC is exactly the same and  you can use G90 or G91 for coordinates,. Just some minor differences.

Update, I added the G91 to the N66 line and it now reads

N66 G28 Z0 G91

Also, It doesn't matter which order I write them on the console, the machine reorders them to that order.

That is a FADAL thing. Delete the entire line and reinsert it. You can also put the G91 on the line before the G28 by itself. I can only see a bit of your program, make sure to switch back to G90 before your next process. Are you using a Z value in your G54 offset? (touching off a known point).

Borg: If you put a canned cycle on each line, the first hole would execute fine. Every location after that would execute twice. (Don't ask me how I know). That's the beauty of the canned cycle. State once. Also the G00 should also cancel the canned cycle. 

Sorry for the delayed response. I had to catch up on the meme thread.🤪

G00 is just a rapid move. Adding it ensures the machine rapids home rather than feeding home if it had a G01 in the lines before the G28.

Your best bet might be to omit G28 entirely and just use G53 Z0.0 I always end my programs by calling up the first tool and a few G53 moves to position the table/tool where I want it:

Impressive, guys....

"Borg: If you put a canned cycle on each line, the first hole would execute fine. Every location after that would execute twice. (Don't ask me how I know). That's the beauty of the canned cycle. State once. Also the G00 should also cancel the canned cycle." 

My CAM program, Aspire, will not use the canned cycle for some reason. It writes out a peck drilling cycle line by line and does it for each position. Not sure why it wont use it. It's a woodworking CAD/CAM but will also do simple metal cutting. 

Hey TM, try it in Aspire if you still have it. It will be a longer program but should work. Unless you want to learn manual programming which is always good to know. 

Somewhere in my office I have all of my notes from programming Fadel and other CNC's and various programs. It's been since about 2003 since I've been in a tool and die shop and for a program that I used to be able to write with no reference help has me confused.  lol

I know I could walk into any shop and hold 0.00005 tolerance on a surface grinder but on a CNC I'd be lost for a week and then struggle for a month. Almost makes me want to hit up the local Juco to take some classes.