[Darth Yoda]

Hi again guys.
I have a program that was produced by blahCAM that produces tons of errors.I am now getting a Sequence number not found error on a Fanuc 18T. the error pops up here:

%
O80
T0505
G50 S800
S500M03
F.006
G00 F.006 G28 U0. W0. F.006
G00 F.006 X-1.25 Z.1369
G71 U.1 R.1
G71 P09 Q38 U.01 W.01 F.006
G00 F.006 X-1.1102 Z.1269
G01 F.006 X-1.0102 Z.0269 .............here............
X-1.0575 Z-.0186
and so on..........

It originally had the N10 N20 etc line numbers but I took them out then put them back in and still got the errors.
What is a sequence number and how do I get rid of this error?

[angelw]

Hi again guys.
I have a program that was produced by blahCAM that produces tons of errors.I am now getting a Sequence number not found error on a Fanuc 18T. the error pops up here:

%
O80
T0505
G50 S800
S500M03
F.006
G00 F.006 G28 U0. W0. F.006
G00 F.006 X-1.25 Z.1369
G71 U.1 R.1
G71 P09 Q38 U.01 W.01 F.006
G00 F.006 X-1.1102 Z.1269
G01 F.006 X-1.0102 Z.0269 .............here............
X-1.0575 Z-.0186
and so on..........

It originally had the N10 N20 etc line numbers but I took them out then put them back in and still got the errors.
What is a sequence number and how do I get rid of this error?

In the second G71 block, there are two addresses that refer to the Start Block Number of the Profile Description and the End Block Number of the Profile Description. These addresses are P and Q respectively. In your example, P09 and Q38 have been used. Accordingly, the control will be looking for Sequence Number N9 for the Start Block and N38 for the End Block. Normally the Start Block will be the Block immediately after the G71 block, and clearly the sequence number has been omitted. It should read "N9 G00 F.006 X-1.1102 Z.1269". As the remainder of your program is not visible, you may or may not have included N38 in the block for the last block describing the part profile.


Regards,

Bill

[Darth Yoda]

Thanks for the reply angelw. That makes sense since the first thing I do is re-sequence the program. It changed the N9 to N90 and N38 to N380.

The reason behind that is the machine operator likes to put notes in between the lines.
Thanks for the answer.

[angelw]

Thanks for the reply angelw. That makes sense since the first thing I do is re-sequence the program. It changed the N9 to N90 and N38 to N380.

The reason behind that is the machine operator likes to put notes in between the lines.
Thanks for the answer.

Sequence numbers are only required by the Fanuc Control in certain instance such as some Multi Repetitive cycles, such as G71, and where a jump to a certain part of the program is required. Apart from that, they consume memory in most instances.

My approach is to only have a Sequence Number at the start of each new tool operation. Its not so critical in a lathe program, as they tend not to be very long, limited to 12 or so tools for the majority of machines, but in a machining centre programs the number of tools used can be considerable. As its uncommon for the sequence of the tools used to follow the sequence of operation, for example T1, T2, T3, T4, etc for operations 1 ,2,3,4, etc respectively, its more likely for the operator to be familiar with the operation sequence than the tool number being used for the operation. Accordingly, if the operation for a particular tool operation is to be repeated, its easier, in my experience, for the operator to identify that its operation number 7 that has to be repeated, rather than know that its tool number 55 that has to be repeated. This can be further confused if spare tools are used in the program. If the 7th operation has to be repeated, then its a simple exercise of searching for N7 and a restart made from there.

In the case of a lathe program, where a G71 roughing cycle may be used, I number the start of each new tool operation sequentially N1, N2 etc, and then use sequence numbers that will be unique in the program, but have some relationship to the sequence number of the tool operation sequence number. For example, if the Tool Operation sequence number is N2, then I'd use N200 and N201 for the P and Q referenced blocks of a G71 cycle. Accordingly, P200 and Q201 will be used in the G71 block. The Program Blocks between the Start Block N200 and the End Block N201 don't require sequence numbers.

Regards,

Bill

[Helman Jr.]

hi,
as you can see below code the block numbers are just given with the contour start and end block numbers of G71 turning cycle. This makes easy to edit, add, remove lines between the contour blocks.

G00 X83.0 Z2.0
G71 U3.0 R1.0
G71 P20 Q30 U0.5 W0.1 F0.27
N20 G42 G00 X30.0
G01 Z-20.0 F0.17
X40.0 Z-40.0
Z-60.0
X50.0 Z-70.0
Z-90.0
X60.0 Z-110.0
Z-140.0
X80.0
N30 G40
G70 P20 Q30

Helman
cnc machining articles