g76 threading help

[panaceabea]

help with threading g76 settings

--------------------------------------------------------------------------------

I need a little help writing the the g76 line to thread with yasnac lx3 controller.

I have been lax in learning basic canned cycles as my other 2 turning centers have really easy to use conversational programing and to date I have not needed to know the how and why , just enter a few parameters , maj, minor pitch and depth per pass and cut the threads.

I have spent the day going thru the 4 pages in the manual that relate to g76 and have written the following which is intended to cut .75x20 tpi . Everything appears OK but it cuts the final pass at a depth of .006" , 2 x my D value.

Is there a way to enter a value for depth of finish pass and any way to callout spring passes (multiple finish passes at the final depth)?

T300
M8
G00 X.755 Z.1
G76 X.7 Z-.75 K.025 D.003 A60 F.05
M9
M30

[extanker59]

I'm pretty sure D is a radial value. Are you saying it's taking .006 on the diameter or DOC. That might explain it if that's what you're seeing.
Yasnac is different. I was expecting to see another G76 line above that one.
On Fanuc, that's where the final pass amount would be.

[panaceabea]

yes its taking .006 off the diameter in the finish pass while all the passes before are aprox .0025 from diameter.
The manual list d as the depth of first pass.
what would I need to add for additional finsh or spring passes

[extanker59]

I'm unsure of your machine. Some only have one G76 line?
Here is an explanation I read on copied a while ago:

G76 P010060 Q00500 R.001 (finish Passes)
G76 P010060 Q00500 R.001 (chamfer Amount At End Of Thread)
G76 P010060 Q00500 R.001 (tool Tip Angle)
G76 P010060 Q0050 R.001 (minimum Depth Of Cut - Radial Value)
G76 P010060 Q0050 R.001 (finishing Pass Depth)


I hope the colors show up...

[extanker59]

Sorry. A full line would look like this:

G00 X.755 Z.1
G76 P010060 Q00500 R.001
G76 X.7 Z-.75 K.025 D.003 A60 F.05
...

If you can't use two lines, maybe it's a parameter for the final pass allowance?

[extanker59]

Here is a link to a much better explanation. (one that doesn't take part of your program and adds it to my explantion)

http://www.rose-training.com/tandp/jun03.htm

[PixMan]

Some older machines use the one-line G76, most newer ones use the two-line version. The one-line is more limited in how it controls the depth of first and last passes, and infeed progression.

With the single-line G76 just put D at the minimal incremental depth you want (probably about.001" or .0005"). Use a smaller value of K to get a bigger "first pass depth" and fewer overall number of passes.

[lyfordln]

The Yasnac controller uses only one line for threading. You can download a manual that explains the various G7-G78 canned cycles at: http://www.yaskawa.com/site/dmcontrol.nsf/536df907f9fe9d5586256c4e0056b851/86256ec30069b63486256de2005ab762/$FILE/TOE-C843-9.20D.pdf

Copy this link, download the pdf file and go to about page 100 and explanations of the canned cycles are there.

Parameter 6206 can be set for final depth of cut

N10T1000
G00G97S500M8
X.500Z.2M3
G76X.435Z-1.0K.035D0100A60F.05
G0X(HOME)Z(HOME)
M01

G76X.(MINOR DIA.)Z-(END OF THREAD)K(HEIGHT OF THREAD)D(1ST PASS, NO DECIMAL POINT)A(INCLUDED ANGLE OF THREAD)F(1/LEAD)

If you need more help, PM me.