[JerryH]

Having a hard time trying to program a Fanuc OT lathe to produce this thread. I'm not sure of the data inputs for G76 cycle. Can someone post a block of code to help me out?

Thanks!

[dcoupar]

Try the example on the attached .pdf

[g-codeguy]

I can give you the correct G76 information for a 1"-11.5 pipe thread Tuesday. I can give you the correct format and explanation now.

G76P000155Q30R(optional & is a decimal)
G76X1.25Z-1.P565Q120R.0344F.087

P in 1st G76 block works in pairs. 1st pair is the number of spring passes, 2nd pair is the pull out (which is .1*F-value in this example), 3rd pair is the compound infeed (55/2=27.5). Q-value is the min. DOC (.003), R.001 would be a finish pass of .001 DOC.

2nd G76 block P= thread height (per side), Q=DOC of 1st pass (per side), R=X-offset amount (per side) to thread correct taper. Start position of Z.5 & end position of Z-1. would =1.5*tan1.78333= R.0467

I have found that the R-value sometimes has to be fudged in order to maintain the correct go/nogo gage depths because of tool pressure.

EDIT: This is for newer controls. Older ones use a 1-block call in the format

G76XZDKFA with D-value not containing a decimal point. If I remember correctly it uses an I-value for a tapered thread.

So G76XZDKIFA Not sure where the I-value has to go, or if it makes a difference.

Here are a couple samples that are used on our machines.

X1.09Z.3M8
G76P000155Q30
G76X1.2365Z-1.15R.0451P700Q120F.08696

OR DEPENDING ON CONTROL

X1.09Z.3M8
G76X1.2365Z-1.15I.0451K.07D120F.08696A50.