Newbie- Need help understanding lathe canned cycles

[chubby hubby]

Greetings All,
I'm taking a CNC class and am having problems understanding the format for G71. This is for external turning on a Haas lathe. My problem is mostly concerning the lines before and after the G71 line. The G71 line itself is easy. Are the preceding and following lines always a G0? If the workpiece is a 5.0 dia and turned down to a 2.0 dia, do I rapid to the largest dia before G71 and rapid the the small dia after the G71? And if there is a radius/chamfer on the face, is a G1 Z0 always used? I hope that I was able to pose this question clearly. Lastly, does this also apply to internal boring? Thanks much in advance. CH P.S. My teacher may know his stuff, but he just can't explain the 'why' behind it.

[Geof]

Look at post #12 in this thread.

http://www.cnczone.com/forums/showth...254#post830254

That post is about boring but turning the OD is the same principle. As you mention you start at the large diameter immediately above the G71 line but after the Q block you don't need anything special.

For chamfers and radii my preference is to G0 to a few to something like Z0.01 and X slightly smaller than the chamfer and then G01 from there.

The G71 can have values in U and W to leave a finish allowance and in this case it is followed with a G70. You can change tool and rpm between the Q line and the G70 but it is important to go back to the original starting point of the G71 before starting the G70.

When you are doing radii for best accuracy normally you need to use tool nose radius compensation which can add a complication on some machines. On early machines the G71 would ignore any compensation commands in the P Q block so it was necessary to use U and W to leave enough material on for a compensated path using G70. Now I have been told on newer machines the G71 will read compensation commands but I have never tested this.

[sinha_nsit]

Originally Posted by Geof I have been told on newer machines the G71 will read compensation commands but I have never tested this.

I would appreciate any information on this, if someone has.

Specifically, has anyone tried 5102#4 (RFC)=1.
From 0i parameter manual:
RFC: For the semifinish figure of G71 or G72 and for a cutting pattern of G73, tool-nose radius compensation is
0: Not performed
1: Performed

[Jhjr]

That is exactly what Geof was talking about. On the last rough pass if your using cutter comp, putting a 1 there will use cutter comp. If you put a 0 there then it won't use cutter comp in the roughing(semi finishing) last pass.

[sinha_nsit]

Does it mean that cutter compensation is not used in roughing passes, but it is incorporated in the last pass (i.e. step-removal pass of type-I cycles).
What happens in type-II cycles, where there is no final pass, since steps are not formed?

[Jhjr]

Yes as I recall it will work on tvpe 2 cycles but it will only compensate in one direction so if you are changing in X plus then minus like a 180 deg radius it will not compensate for the back of the tool just the front or visa-versa. Shouldn't matter to much on a rough pass though. HTH

[sinha_nsit]

Logically it should compensate in both directions. Compensation on one side is meaningless.
Parameter manual does talk about compensation in roughing cycles, but operator's manual says that compensation cannot be used in these cycles. We have to interpret Fanuc manuals ourselves.

[mousongie]

Hi;

Before starting i would like to let you know that the principe of turning is almost identical to the one of boring.

Now lets go to the point.
1) On my opinion i always rapid the tool to the diameter of the stock plus twice the amount of the tool radius. in your case lets you are using a roughing tip of 0.8 radius(this is a metric quote), my line before G71 will be as follow;

G0 X6.6: 5.0+(0.8*2)=6.6
G71 U1.5 R1.0


2) When it comes to the line after G71 i do apply the same principe. Lets say when the contour is at the end 2.0 in your case ,i will rapid the tool to X3.6 2.0+(0.8*2), but this may not be important because like on Fanuc (i dont know others controls) ,after the last line of G71 the tool will rapid to the starting point (ie) X6.6 before proceding directly or indirectly to the tool change position as specified in the program format.

3) When a chamfer or radius is needed,it obvious that the tool must touch the face of the workpiece which is Z0


Remember that all my numbers are in metric mode.

Should you have more questions please fill free to contact me.