YASNAC Program Issue

[Bubby44]

Hello,

I'm running a Kia KT-21 with a Yasnac LX-1 Interface. I'm trying to proof a program and it will not process the canned cycles I have written. I've been through it and based on other programs that have been run through the machine, I should not have a syntax error. I will run up to the G71 code of the canned cycles and then stop it dead in its tracks, or it will skip these lines entirely and continue on. The rest of the program runs through smoothly. Any Suggestions are greatly appreciated.

Thank you

Jake

Similar Threads:

• Need Help!- yasnac controller program getting scrambled. not sure why
• Yasnac to laptop OK, but getting program into machine, not happening
• Need Help!- YASNAC LX-3 on METHODS Slant 50 Rapid Traverse issue!
• Need help restarting a program at a tool with a Kia Turn 15 w Yasnac LX3 controller
• Cutter comp issue Yasnac MX3

[machinehop5]

your G42 maybe on the wrong line. try it on line 10. Also, is your Tool Tip position correct?
CNC Lathe Tool Nose Radius Compensation - CNC Training Centre

[Bubby44]

your G42 maybe on the wrong line. try it on line 10. Also, is your Tool Tip position correct?
CNC Lathe Tool Nose Radius Compensation - CNC Training Centre

I believe the tool tip position is correct. This system uses G50 codes for positioning, which I'd never dealth with before at my previous shop. The tool approach looks correct for the rest of the program.

[machinehop5]

I should not have a syntax error.

Line 6 & 42 looks odd to me..."G50 X5. Z5." is this possibly the syntax you spoke of ?

[Bubby44]

your G42 maybe on the wrong line. try it on line 10. Also, is your Tool Tip position correct?
CNC Lathe Tool Nose Radius Compensation - CNC Training Centre

I tried moving the G42, it just skipped over the cycle again.

Line 6 & 42 looks odd to me..."G50 X5. Z5." is this possibly the syntax you spoke of ?

That is the preset that BobCAD generated, we changed the X and Z to the position of the the tool at zero relative to the work. Neither of us have worked with G50 positioning before, this is our first time using this lathe. Since no one uses G50 anymore, the few instructional's I've read and videos I've watched haven't been all that clear or helpful.

[machinehop5]

Try changing Line 6 from G50 X5. Z5. to G92 X5. Z5....and change Line 42 from G50 Z5. to G92 X5. Z5. ......... add a G90 on Line7 and on Line43

G50 is just for Spindle RPM max... How to use G50 on a CNC lathe - CNC Training Centre

[Dualkit]

Not the same generation but I had a Yasnac X3 that was real strange when it came to cutter comp. To get it to work right every time it had to be on it's own line of code all by itself.

[BlueChip]

My recommendation ... take the G42 out of the canned cycle completely.
Some generations don't accept G41/G42 in the canned cycle ... it's roughing anyway, any TNR error will be taken out during finishing ... save yourself a lot of headaches.
To include it in finishing ... activate G41/G42 before you command the G70.

Since this generation didn't have "geometry" offsets ... it used G50 to preset the tool position.
Sorta like geometry offsets ... except the values are written directly into the program.
G50 is the distance and direction from the tool tip at the index position to the X0/Z0 position on the part.
When the G50 is read ... the position display gets preset to the X/Z values on the G50 line.
So if you have G50 X2.0Z2.0 ... the machine will think that it is at X2.0 Z2.0 ... and then if you command G00X0Z0 ... the tool move -2.00 in Z and -1.0 (radius) in X to get to 0,0.
Since very tool sticks out of the turret differently ... every tool has it's own G50 position.
Old school ... but like I said sorta think of it as new school geometry offsets.

Also ... G50 can be used as a spindle restraint ... so G50S2500 will insure the machine spindle never goes beyond 2500 RPM.

Hope this helps ....
Check out out Real World Machine Shop Software at
https://www.KentechInc.com

[Bubby44]

My recommendation ... take the G42 out of the canned cycle completely.
Some generations don't accept G41/G42 in the canned cycle ... it's roughing anyway, any TNR error will be taken out during finishing ... save yourself a lot of headaches.
To include it in finishing ... activate G41/G42 before you command the G70.

Since this generation didn't have "geometry" offsets ... it used G50 to preset the tool position.
Sorta like geometry offsets ... except the values are written directly into the program.
G50 is the distance and direction from the tool tip at the index position to the X0/Z0 position on the part.
When the G50 is read ... the position display gets preset to the X/Z values on the G50 line.
So if you have G50 X2.0Z2.0 ... the machine will think that it is at X2.0 Z2.0 ... and then if you command G00X0Z0 ... the tool move -2.00 in Z and -1.0 (radius) in X to get to 0,0.
Since very tool sticks out of the turret differently ... every tool has it's own G50 position.
Old school ... but like I said sorta think of it as new school geometry offsets.

Also ... G50 can be used as a spindle restraint ... so G50S2500 will insure the machine spindle never goes beyond 2500 RPM.

Hope this helps ....
Check out out Real World Machine Shop Software at
https://www.KentechInc.com

Removing the G42 entirely didn't change the outcome, still got G70-76/G72-78 error. It is good to know that isn't the problem though.

I did alter my G50 coordinates to reflect your instructions and the machine moves exactly where I want it, but it still won't read through those canned cycles.

Try changing Line 6 from G50 X5. Z5. to G92 X5. Z5....and change Line 42 from G50 Z5. to G92 X5. Z5. ......... add a G90 on Line7 and on Line43

G50 is just for Spindle RPM max... How to use G50 on a CNC lathe - CNC Training Centre

Changing the G50's to G92's got me 030: Prog Error (F/E)

Adding G90 to line 7 and 43 caused program error 104 (Double Addrs)

[machinehop5]

I was just looking around the Net...
https://www.cnczone.com/forums/fanuc...71-issues.html

[BlueChip]

Couple more things to try ...

(1) When using the G71 you first move the machine to point A ( these are the coords the tool is at just before you call the canned cycle ) ... in your case the last X is 1.11 and the last Z is .8187. You need to return to that point when the last N ( Q ) number is executed. In your program that doesn't happen. Make sure that X is 1.11 and Z is at .8187 before N19 ... so N18 should be G01 Z.8187 and N19 should be G40 X1.11.

(2) On a Fanuc control an X and Z move on the P (N) line turns on Type II G71 canned cycle where non-monotonous shapes can be machined. This is an option on some Fanuc controls and will generate an alarm if the option isn't there. Maybe something like that here. I would make try taking the Z move out of the line ... see what happens.

Hope this helps ...
Check out our Real World CNC / Machine Shop Software at
https://www.kentechinc.com

[Bubby44]

Couple more things to try ...

(1) When using the G71 you first move the machine to point A ( these are the coords the tool is at just before you call the canned cycle ) ... in your case the last X is 1.11 and the last Z is .8187. You need to return to that point when the last N ( Q ) number is executed. In your program that doesn't happen. Make sure that X is 1.11 and Z is at .8187 before N19 ... so N18 should be G01 Z.8187 and N19 should be G40 X1.11.

(2) On a Fanuc control an X and Z move on the P (N) line turns on Type II G71 canned cycle where non-monotonous shapes can be machined. This is an option on some Fanuc controls and will generate an alarm if the option isn't there. Maybe something like that here. I would make try taking the Z move out of the line ... see what happens.

Hope this helps ...
Check out our Real World CNC / Machine Shop Software at
https://www.kentechinc.com

I took the Z move out of line 10 and it final ran through. Had a couple bumps the rest of the program, but nothing major. Thank you so much for helping me sort this out!

[machinehop5]

define g41 vs g42 path...maybe the problem...front or rear tool charger....upside down or inside out cw or ccw realtime g41 gfourtwo....you make the call Programmer

Never give up, to simple problem