Any idea why this roughing canned cycle won't work?

[Darc]

The machine is a Fagro 800T lathe (Damn old, but not bad otherwise)
It keeps giving me the error code 021 see manual, for the love of god I can't get this to work.
I've attached the relevant parts of the manual.
Thanks

Fagor 800T Info

G90 G71 G40 G95 F2.0
T06
G96 S1100
G92 S2350
M04
G00 X9.0
Z1.0
G68 P0 = K9.0 P1 = K1.0 P5 = K0.6 P7 = K0.3 P8 = K0.0 P9 = K0.2 P10 = K1.0 P13 = K190 P14 = K320
G40 G00 X60.0
M05
M30
N190 G90 G01 X4.7 Z1.0
Z0.0
X5.70 Z -0.5
Z -8.0
X6.3 Z -8.3
Z -47.01
X5.5
Z -47.58
X4.4 Z -49.54 I12.82 K -49.54 (R4.21)
Z -63.83
G02 X5.71 Z -66.29 I14.18 K -63.84 (R4.89)
G01 X7.3 Z -67.67
G00 X12.0
N320 Z1.0

[WayneHill]

Originally Posted by Darc The machine is a Fagro 800T lathe (Damn old, but not bad otherwise) It keeps giving me the error code 021 see manual, for the love of god I can't get this to work. I've attached the relevant parts of the manual. Thanks Fagor 800T Info G90 G71 G40 G95 F2.0 T06 G96 S1100 G92 S2350 M04 G00 X9.0 Z1.0 G68 P0 = K9.0 P1 = K1.0 P5 = K0.6 P7 = K0.3 P8 = K0.0 P9 = K0.2 P10 = K1.0 P13 = K190 P14 = K320 G40 G00 X60.0 M05 M30 N190 G90 G01 X4.7 Z1.0 Z0.0 X5.70 Z -0.5 Z -8.0 X6.3 Z -8.3 Z -47.01 X5.5 Z -47.58 < G02/G03 ??? > X4.4 Z -49.54 I12.82 K -49.54 (R4.21) <G01 ???> Z -63.83 G02 X5.71 Z -66.29 I14.18 K -63.84 (R4.89) G01 X7.3 Z -67.67 G00 X12.0 N320 Z1.0

G02/G03 and G01 missing ?

If it is anything like the Fanuc roughing patterns, the toolpath must follow in a set direction and not "backup" or "undercut" on itself. (Bad description).

[MILLMANM]

Darc
I SEE 2 PROBLEMS

1 IS A CHANGE IN X DIRECTION
X5.70 Z -0.5
Z -8.0
X6.3 Z -8.3
Z -47.01
X5.5
Z -47.58
MOST CAN CYCLES WILL NOT CHANGE AXIS DIRECTION
HAAS LATHE WITH YASNAC CONTROL WILL DO THIS MOVE

2 MISSING G02
G01 Z -47.58
G02 X4.4 Z -49.54 I12.82 K -49.54 (R4.21)
G01 Z -63.83


YOU CAN JUST PROGRAM THE GEOMETERY
WITHOUT A CAN CYCLE AND SEE IF IT RUNS
OF COURSE OFFSET TOOLS OR REMOVE STOCK

IF THIS WORKS YOU CAN WRITE THE ROUGHING PROGRAM LONG HAND


G90 G71 G40 G95 F2.0
T06
G96 S1100
G92 S2350
M04
G00 X9.0
Z1.0
G68 P0 = K9.0 P1 = K1.0 P5 = K0.6 P7 = K0.3 P8 = K0.0 P9 = K0.2 P10 = K1.0 P13 = K190 P14 = K320
G40 G00 X60.0
M05
M30
N190 G90 G01 X4.7 Z1.0
Z0.0
X5.70 Z -0.5
Z -8.0
X6.3 Z -8.3
Z -47.01
X5.5
Z -47.58
X4.4 Z -49.54 I12.82 K -49.54 (R4.21)
Z -63.83
G02 X5.71 Z -66.29 I14.18 K -63.84 (R4.89)
G01 X7.3 Z -67.67
G00 X12.0
N320 Z1.0

[Darc]

Thanks for the response Millman.
I tried your suggestion of making it go 1 way, but it still comes up with the error 21.
I wrote this program and it still won't work. well it's got me stumped.

G90 G71 G40 G95 F2.0
T06
G96 S1100
G92 S2350
M04
G00 X9.0
Z1.0
G68 P0 = K9.0 P1 = K1.0 P5 = K0.6 P7 = K0.3 P8 = K0.0 P9 = K0.2 P10 = K1.0 P13 = K100 P14 = K200
G40 G00 X60.0
M05
M30
N100 G01 X5.0
Z-10
X8.0
Z -20.0
X12.0
Z -30.0
N200 X15.0

[TEXASLEADH]

On What Block Does It Error? (021)
Will The Program Load From Disk Or Rs-232?
Are You Writting This Program On A Pc?
All Fagors I Have Ever Ran Required Line Numbers On Every Block.
Their Manuals Have A Lot Of Errors In Them. It Takes Alot Of Thanking To Figure Out How Or What They Were Thanking And How To Apply It.
Just Like Your Pdf File And Their Examples In My Manuals Don't Show P10 But It Is Required.

[DareBee]

Just a touch off topic - but I have a new lathe with a Fagor 8040T control, and I love it.
The conversational programming is EXTREMELY simple.
I haven't bothered to check what sort of code output it makes.
Maybe once I am done running this job I will copy the code from a straight turning block and post it for you, don't know if it will help, but what the hey.

[Darc]

I have written the program on both a pc and on the machine, our machine is very sensitive about incorrect parameters, it will not go across from the pc if something isn't correct.
I think the error was coming up on line the G68 code is on.
Yeah sorry I removed the line numbers to make it easier to read, I think it made it harder.

[Unimatrix]

We have a lathe with the fagor 800t controller, too!
Do u have an ISO Programm running? Or do u have examples for ISO programms? We have big troubles with this controller!!

[tmax]

I've been getting calls for this for 9 years. If you turn the page for G68 it explains this:
5. The pattern can be made up of straight lines and arcs. All the blocks of pattern
definition will be programmed with cartesian coordinates being mandatory to
program the two axes in absolute, otherwise, the CRT will display error 21. If arcs
are included in the definition, they must be programmed with the center’s I,K
coordinates, referred to the arc’s starting point and with the relevant sign. If
functions F,S,T or M are programmed in the definition, they will be ignored except
for the finishing pass. No polar definitions can be used.

A block in a profile must be as follows:
G1XZ
G2XZIK

Tom Maxwell
Fagor apps engineer

[tmax]

Hey Unimatrix,
The 800T is a bit tricky to use. You can only run one iso program, 99996. It's programming is very similar to 8025, but the cycles are a little different as shown it's programming manual. If you have Ver. 6.6 there is a way you can get the cnc to convert a conversational program to P99996 using simulation.
3. GENERATING AN ISO-CODED PROGRAM
With this CNC, the ISO code (low level) for an operation or a part-program may be generated.
To use this feature, machine parameter "P623(2)" must be set to "1".
This ISO program always has the number: 99996 and can be stored either at the CNC or at a PC.
Program 99996 is a special user program in ISO code and can be:
Generated from an operation or a part-program.
Edited at the CNC itself via menu option: "Auxiliary Modes - Edit program 99996"
Loaded into the CNC after being generated at a PC.
Generating the ISO program (99996) at the CNC.
This CNC has 7 K of memory space to store program 99996. If the generated program is larger than that, the CNC will issue
the relevant error message.
To generate program 99996, proceed as follows:
* If it is an operation, select or define the desired operation.
* If it is a part-program, select the desired one in the part-program directory and place the cursor on its header ("PART 01435".
A listing of the operations it consists of must appear).
* Press the keystroke sequence: [AUX] [7]. The CNC will show the graphic simulation screen.
* Press . The CNC starts simulating the part and generating its ISO-coded program 99996.
* When done with the simulation, program 99996 stored in CNC memory will contain all simulated blocks in ISO code.

This should give you an idea of the structure of the code.
Hope this helps,
Tom Maxwell
Fagor apps engineer

[Unimatrix]

U mean the controller can show me the ISO-code of an cycle?

And why does the controller activate the radius-correction only at the last operation? We have so big troubles to make a radius with a large turning tool!

And how do I knwo which version i have?

[little bubba]

Just guessing but if this is the same as an 8025, your P0 & P1 should be the first point in your profile. Then the P13 P14 should be the contour of the rest of your profile. Therefore P0 =K9. is larger than the first point in your profile, when I check a program I check to make sure that the X is always going in one direction and the Z the other. The point you moved your tool to before calling the canned cycle determines the outer X and Z points. So simply take the first point of your profile and make that your P0 and P1, then start your P13 P14 profile at the second point of your profile. I hope this helps.