[idtkid]

Bear with me, I am very new to using industrial machines so im sure my error is very obvious.

Pasted below is the beginning part of my ~2000 line program, upon trying to run this in single block mode I get a syntax error, can you spot it?
(RhinoCAM posted this code, my Fanuc 21m controller adds a semicolon character at the end of each line)

O0001
%
N0005G0 G91 Z0
N0010G0 G90 G17 G20 G40 G80 G90 G94 G64
N0015G0 G90 G54 X0 Y0
(2 1/2 Axis Facing)
N0020 T3 M6
N0025 M8
N0030 G90 G1 X-0.8875 Y0.6125 F200. S5000 M3
N0035 G90 G43 Z0.25 H0
N0040 Z-0.0625 F60.
N0045 Y2.75
N0050 X-0.8753 Y2.8744
N0055 X-0.839 Y2.994
N0060 X-0.7801 Y3.1042
N0065 X-0.7008 Y3.2008
N0070 X-0.6042 Y3.2801
N0075 X-0.494 Y3.339
N0080 X-0.3744 Y3.3753
N0085 X-0.25 Y3.3875
N0090 X3.25

[dcoupar]

What is the alarm number?

[dcoupar]

Could be the H0. I would guess it should be H3.

[dcoupar]

I would also think you want N0005 to be G0 G91 G28 Z0 to take Z up to it's home position.

[idtkid]

Error is: 9 N 0 SYNTAX ERROR (i have changed H0 to H3, what does this do?)

[dpuch]

Error is: 9 N 0 SYNTAX ERROR (i have changed H0 to H3, what does this do?)

G43 H# activates the tool length offset for tool # in this case tool 3
dcoupar's other comment looks like a good change as well.

Which line is it stopping on? You should be able to look at the line after the error pops up. If you have a problem with that, try using single block until you get the error. That should narrow it down greatly.

Edit: Doh, your second line is % that usually marks the beginning and end of a g-code file.

[MysticMonkey]

EOB goes before the comment

[kazikw]

First what I see isunnormal lookig line NG90G43Z0.25HO
I think firs should be H value than Z value.
Tray this way NG90G43H3Z0.25
If not work let me know

[Superman]

O0001
%
N0005G0 G91 Z0

The % is not part of NC language

it is used with communication software for start and end of transmission

This is the only source for the syntax error. It is to be the only code on #1 line ( some controls use it at the end of the filename string on the 1st line--Okuma's ) or deleted, it should also be the last character in the file

All other items mentioned will not cause the machine to not cycle start

[MysticMonkey]

Sorry to nitpick

But having % mid way through the program doesn't cause the Syntax error.

Not having the program number after the % at the beginning of the program will cause an error.

When the data is sent over RS232 it uses the O program number after the % to name it's self.

[sinha_nsit]

H0 cancels the tool length compensation, like G49.

Like many others, I am not comfortable with % sign. Remove it and run the program in single block to find out where exactly it alarms out.

[dpuch]

Sorry to nitpick

But having % mid way through the program doesn't cause the Syntax error.

Not having the program number after the % at the beginning of the program will cause an error.

When the data is sent over RS232 it uses the O program number after the % to name it's self.

Actually on our machines 15,16, 16i They all default to O0000 if there isn't a program number, but that may be a parameter option. Anyhow it's almost certain the % should not be there. A question is it there in the file, or somehow on the control? And again which line is it stopping on in single block.

[idtkid]

Thanks guys, removing the first % sign fixed the prob, I forgot to try placing it before the program number to see if that would cause it as well. Appreciate the help!

[machinist_1]

I have the 18i on a new FADAL. My tool call has to be M6 T#. Where are you alarming out at, what line? Line # 5 shouldn't be there. At least not like that. Add a G28. But when you make a tool change, your Machine will return to Z0 without line # 5. Line 35, your G90 should be GO instead. H should be the same as the tool #. And put that percent sign at the start and end of the Program.

[Dan Fritz]

Glad you found the problem, but there's one other thing to watch out for:

Your 21i is apparently set to accept ASCII characters instead of ISO. Most older Fanuc models would have thrown a TH (Tape horizontal) alarm when reading your comment. Lower-case letters are legal in ASCII but not in ISO. On the 21i, there is a parameter for this (I think it's a bit in parameter 100)

[skullworks]

Actually on our machines 15,16, 16i They all default to O0000 if there isn't a program number, but that may be a parameter option. Anyhow it's almost certain the % should not be there. A question is it there in the file, or somehow on the control? And again which line is it stopping on in single block.

Technically I was told that program o0000 is assigned to the MDI buffer.