Learn Fanuc CNC Lathe Programming.
Call at 614-888-8466 with any CNC programming questions.
Ask for Heinz.
Fanuc CNC lathe programming knowledge:
Learn Fanuc CNC lathe programming from the examples on this website.
To learn the detailed method of all parts of Fanuc CNC lathe
programming from my CNC DVDs, look at the
Fanuc DVDs on the main website below: http://www.doccnc.com
Learn more and earn more!
Are you an operator trying to learn more and get a better paying job
as a programmer?
Look at the video outlines and be honest about where you are lacking in CNC skills, buy
the proper DVD, learn, and put your skill to work tomorrow.
Do you need to get a new or used CNC Machine into
Did you buy a used CNC lathe or mill and need to learn to program your investment, make
parts efficiently and pay for your investment?
The DVDs cover the detailed method of programming Fanuc-Yasnac from 1980 to today.
Watch, listen and learn and you should be making profitable parts soon.
Should you be more productive and efficient?
Are you an owner or manager of a CNC shop and you feel that your machines could be a lot
Most likely, you could be 15% to 20% more efficient.
Efficient CNC shops are far and few between, follow the experiences I gained by
training hundreds of shops around the US and Canada, all of which you will lern
from my DVDs.
If you do, you can be sure your shop will become a lot more efficient.
Here is a picture of a recent CNC training
job I did for Bradley's Motors in Corpus Christi, TX.
This is the first part we made on a large CNC lathe with the Fanuc control.
The machine was sold by Industrial Machinery at www.industrialmachinery.com
On all CNC controls, X is the diameter of the part.
A diameter of 4" is written as X4.0 (This was not always so, a lot of
European machines used Radius for X.)
Z is the absolute length dimension.
The finish face of the part is set to be Z zero.
Dimensions are written and entered into the control with decimal points, Z- 2.0 represents a
distance of 2.0" past the face of the part toward the chuck.
The motions available:
G0=Rapid (Max available, can usually be overridden.)
G1=Linear feed (Needs feedrate)
G2= Circular CW
There are a lot more G codes, they will be explained as they appear in the following
If you need any help with any lathe or mill programming
question, call me at 614-888-84676 or send an email to email@example.com
Fanuc Lathe Program Example.
Part is 2" OD, will be finish faced with OD skin cut taken.
N1G50S2500(The G50 sets up safe max speed.)
N2T0101(Tool index to position 1, use tool offset 1 to set tool and to change part size.)
N3 G96S650M3(G96 is Constant Surface Feet, S is amount, M3 is spindle on CW.)
N4G0X2.1Z0(Rapid to above OD and face of part.)
N5G1X.5F.006(Face to .500 at a feed of .006 per rev.
N6G0X2.0Z.1(Rapid to 2" diam. and clear part on way up.)
N7G1Z-1.0F.001(Cut left at F.001.)
N8G0X6.0Z6.0(Rapid to clear for loading new part, newer controls do not need tool offset
N9M30( Ends program, resets memory to start.)
Usually coolant is used, M8 is on, M9 is off.
Fanuc CNC Lathe program using Noseradius
Before using this program, make sure to put size of
noseradius into R in the Offset register, also the number describing the
tool into T, usually 3 for OD tools and 2 for boring bars.
N1 G50 S2000 *
N3 G96 S500 M3*
N4 G0 G42 X2.0 Z.1 M8* (Set comp to the right)
N5 G1 Z-1.0 F.008*(Comp is calculated by control where needed based on size of
noseradius, shape of part and the tool shape)
N6 X2.5 Z-1.7*
N9 G0 G40 X6.0 Z6.0 *(Make sure to cancel comp)
The typical Canned Cycles to make programming a lot easier:
G71 does turning-boring with very little info.
G76 cuts a thread, straight or tapered, also with very short, basic info.
Example: G76 Threading Cycle in 2 line format for OT and later controls.
2" diameter, 20 Threads per Inch, Mild Steel.
N1 G50 S1500*
N3 G97 S700 M3*(Speed for threading, always in RPM)
N4 G0 X2.2 Z.2 M8*(Rapid to above part, .2" from face)
N5 G76 P021060 Q20 R5*(The first 2 digits in P represent the amount of finish
passes, the next 2 are the pullout distance at the end of the threading motion, expressed in tenths
of revolutions, the 60 is the angle of the tool)
N6 G76 X1.94 Z-1.0 P300(total thread depth) Q150(depth of first cut) F.05*
R if needed is the amount of taper over total distance in thread motion.
The P value is figured by taking the F-value times the constant of .6, once
figured you also have the X value.
N7 G0 X6.0 Z6.0 M9*
The G71 turning-boring cycle:
This is a simple example, it turns a 4" diameter piece of 1018 steel
down to a 2" diameter, 1" back from the face of the part.
N1 G50 S2500(Max speed)
N3G96 S600 M3(Speed in SFM for 1018 Steel)
N4 G0 X4.0 Z.1 M8(Rapid to OD of part, .1" away
from face, turn coolant on)
N5 G71 U.15 R.02(U=cutting depth, R= pullaway
distance after each cut)
N6 G71 P7 Q9 U.05 W.005 F.015(P7 tells the control to
look at N7 and Q9 to look at N9, this is how we give the motions describing the part.
U is the amount of stock left for finishing on the OD,
W is the amount left on the shoulder.
N7 G0 X2.0
N8 G1 Z-1.0
N10 G0 X6.0 Z6.0 M9(Rapid back to a position clear of
Call or E-Mail for any CNC Lathe or Mill questions.
614-888-8466, ask for Heinz.