[DocHod]

Hi all I have a question about roughing a 1/4 rad.concave profile , all I wanted to do is rough and finish a 1/4 rad. groove in a 1"dia. round bar this is being done on a Viper lathe with a fanuc 21i controller , it wants to try and take the full rough depth of the radius at one time I have the program that I used and ended up just using large x+ wear offset and decreasing it after every complete cycle to get what I needed and the radius turned out fine but there has to be an easier way. I may be using the wrong canned cycle don't know for sure ? I have the program listed below any help I would be grateful.
O9997(OD CONCAVE .25 RAD.)
G0G28U0.
T0303(.170 RAD.TOOL ROUGH)
M91(main spindle call)
G92S1400(max. r.p.m.)
G96M03S575
G0X1.1Z-.92
G71U.05R.02
G71P1Q10U.02W.005F.008
N1G1X.83F.01
G2X.83Z-1.25R.08
N10G1X1.1
G0Z-.92
M1
T0303(.170 RAD. TOOL FINISH)
M91G96
M03S600
G0X1.1Z-.92
G70P1Q10
G0G28U0.
Z5.
M91M5
M30

[CNCRim]

From what I know, since you do a pocket like, U parameter on the second line should be U0, otherwise it cut too much on one side. However, I used to do the similar pocket type on Mazak(Mitshubisi control in G-code) and I was able to program U.005 W.005 and the machine somehow knew and leave .005 all the way around without overcut.... so my conclusion is whatever flow you boat go with it.

[dcoupar]

First thing I see is the N1 line needs and X and Z move to tell the control that it's a Type II (non-monotonous) roughing cycle (X goes -, then goes +).

Newtexas2006 is correct, somewhat. Actually, you want the W to be 0 so it doesn't overcut on the back side of the tool. The U0.02 is ok.

Also, not having a blueprint in front of me, it seems your X start and endpoint of the arc are off by half... try this one:

%
O9997(OD CONCAVE .25 RAD.)
G0G28U0.
T0303(.170 RAD.TOOL ROUGH)
M91(main spindle call)
G92S1400(max. r.p.m.)
G96M03S575
G0X1.1Z-1.09
X1.01
G71U.05R.02
G71P1Q10U.02W0F.008
N1G1X.66W0F.01
G2X.66Z-1.25R.08
N10G1X1.01
G0X1.1Z-1.09
M1
T0303(.170 RAD. TOOL FINISH)
M91G96
M03S600
G0X1.1Z-1.09
X1.01
G70P1Q10
G0G28U0.
Z5.
M91M5
M30
%

[DocHod]

I can't use the W on line 1 of the program for some reason the machine builder decided to use W as the sub spindle axis so when I tried it it did what I expected it to do it moved the subspindle axis (W) to W 0. at a feed rate of .01/rev. of the main spindle and the radius profile that I wanted to rough just wanted to cut all the material in one pass. Any other suggestion other than just calling the machine tool company that we bought it from? and yes the profile comes out were I want it to with the program I posted.

[Chris D]

There are two types of roughing cycles using the G71 code. The standard version only allows you to start at a small diameter and the diameters MUST progressively get bigger as you move into the part (opposite for boring).

FANUC has an optional roughing cycle that allows you have intermixed diameters of smaller and larger diameters along the roughing cycles length. You need this optional cycle.

Chris

[Geof]

I looked at your first post a couple of days ago and didn't respond because I program on Haas. But after reading it through in more detail I have a question; where is your D, the cut increment, in the G71 line? Or does Fanuc use a different letter to label the cut increment?

[dcoupar]

Well, then, try this:

G0X1.1Z-1.09
X1.01
G71U.05R.02
G71P1Q10U.02Z-1.09F.008

[Kai_DK]

You can have another problem.
Fanuc sometimes cannot work out the correct circular interpolation if you have motion on more than 90 degress.
Split the contour in 2, g2 xxx zzz rrr + XXX ZZZ rrr, and maybe put a G1 motion to go to position inside your cycle.

[DocHod]

dcoupar I will try your suggestion tomorrow if I get a chance with the second G71 line using the Z-1.09.

[DocHod]

Geof the first G71 line with the letter U=the depth/pass the R is the amount of retract after the rough pass , the second G71 line U= amount of finish on the X and the W= amount left for finish on the Z , hope this clarifies this for you. G71U.05R.02
G71P1Q10U.02W0F.008

[DocHod]

dcoupar , I tried what you posted on 12-3 and it is still a no go I'll have to try calling the machine tool company we bought it from , I know there is a couple of other ways of doing it but man it would be nice just to use the G71 cycle.

[dcoupar]

Please post the current program. Maybe it's something obvious.

[theemudracer]

OT:

we also have had a viper for 2 years in production. We are selling it and getting a real machine. Our experience is .........VIPER SUCKS

I know this has nothing to do with the current post. Im just venting...LOL