tool comp or look ahead problem

so i got a program and have
G41 Y1.0000 D1 F20.
G4 P20000 (delay of 20 seconds)
;
;
X10.
G40 Y2.0
.
and i put the 2 blank lines in to make it easier to read but when i see distance to go i see a .001 or .002 on Y axis when it is suppose to only move in X10.
.
i remove blank lines and it moves straight in X and no change in Y
.
only thing i can think of is cnc looks ahead 2 or 3 lines and if it does not see the next coordinate move in 3 lines it does something off with tool comp.
.
i just wondered if it is a fanuc 15 thing or do all cnc do this when too many blank lines are between G41 line and the G40 line

Before computer generated G code we were always taught to "comp on" then "comp off", meaning
position the tool X and Y then G41 to your location and always at a right angle, G40 the same way.

X 1.00 Y.25
G1Z-.5
G41X.75
Y-1.
G40X1.00

The x on and x off move distance would be dependent on coding to center of tool or edge

Omega said:

Before computer generated G code we were always taught to "comp on" then "comp off", meaning
position the tool X and Y then G41 to your location and always at a right angle, G40 the same way.

X 1.00 Y1.00
G1Z-.5
G41X1.25
Y-1.
G40X1.

The x on and x off move distance would be dependent on coding to center of tool or edge

Click to expand...

.
my point is blank lines causing a problem. the program works ok without too many blank lines between the G41 and G40.
...... i am not talking about tens of thousands of successful programs only about too many blank lines causing a tool comp problem. i saw it on the distance to go screen in single block mode. it has nothing to do with the programs and everything to do with the extra blank lines as the problem went away when i removed the blank lines.
.
the cnc control high lights the lines ahead that it is reading usually a line or 2 ahead of current line being done. i have used a G4 pause after a G41 right angle move thousands of times before. i usually do not add extra lines before now
.
the programs often have
M9
G53
extra in program merely to fill the read ahead buffer with relatively unimportant stuff. obviously you do not need to give a M9 or turn coolant off more than once. G53 with nothing else on line does nothing and next line it returns to what ever work coordinate was active like G55
.
i am not sure if more modern cnc looks ahead more lines in a program
.
the error was only a .001" in Y in over 50" of X movement. if i was not looking for it it could have gone unnoticed. i used wear comp so tool radius comp is usually small often less than .010"
...... it might have been tapering off tool radius comp to zero in Y by the end of the 50" X move

..or maybe the wear # is bigger than the first comp on move ?

on a Fanuc control if you have two lines of info in a row that do not contain axis motion tool comp will not function as normal, this is right in the Fanuc documentation. It will normally result in accumulation errors

Tom said:

on a Fanuc control if you have two lines of info in a row that do not contain axis motion tool comp will not function as normal, this is right in the Fanuc documentation. It will normally result in accumulation errors

Click to expand...

And people wonder why Fanuc sucks. They haven't updated their crap controls in decades.

tool comp

Tom said:

on a Fanuc control if you have two lines of info in a row that do not contain axis motion tool comp will not function as normal, this is right in the Fanuc documentation. It will normally result in accumulation errors

Click to expand...

.
yes i saw in the manual that it is not recommended to have 2 non movement lines in a row when tool comp is active and the manual tries to explain what happens.
.
easier to not have 2 non movement lines in a row rather than try to figure out exactly what it will do
.
i watched program check screen yesterday when it sees G4 pause it reads a 2nd line ahead. must be a limit of 2 lines read ahead looking for a tool movement
.
G4 P20000 M8 .....combining some items on same line works usually.