Repeditive O.D. Machining

[wevz]

I'm sure someone can help with this. I need to remove 14.0 mm from a bar stock. I want to remove .5mm on a pass. I always do this the hard way with a long program. I'm sure there's a way to do this with a macro. Can anyone explain this to me? Thanks!

[Geof]

Does your machine not support G71, G70 roughing and finishing cycles?

[wevz]

yes my machine suppots this, iv'e just never used it. I have to go from
20.mm to 6.mm diameter. cutting 40.mm length. 2400 rpm at .075 feed. Like I said i never used a G71 and it looks confusing in the book. Probably because
I don't use incremental positioning.

[Geof]

Originally Posted by wevz yes my machine suppots this, iv'e just never used it. I have to go from 20.mm to 6.mm diameter. cutting 40.mm length. 2400 rpm at .075 feed. Like I said i never used a G71 and it looks confusing in the book. Probably because I don't use incremental positioning.

I will agree most Manuals manage to make things look much more confusing than they are. But your machine is unusual if you need to use incremental for G71. The D value that is put in the G71 is incremental radius measure and the U and W for the finish allowance are both incrmental measure but the program block selected by the P and Q can be all absolute.

You would set your start X and Z; if Z zero is taken at the end of the stock then these would be X20. Z0.5 to give a little Z clearance.

Your feed (F) is .075 and you want to take off 0.5mm per pass so D is .25 so your program would have something like this:

Choose tool
Start spindle
G00 X20. Z0.5 (Move to start position)
G71 P3 Q4 D0.25 U0. W0. F0.075
N3 GOO X6.0 Z0.0
N4 G01 Z-40.
Rest of program

This format is for Haas operating in Fanuc mode, I think some machines require you to put entries on two separate lines but the principle is the same.

[wevz]

Thank you. I will try this in the morning. This will cut my so much writing out of my program. I have always done it the hard way because i didn't know any better.

[g-codeguy]

Originally Posted by Geof I will agree most Manuals manage to make things look much more confusing than they are. But your machine is unusual if you need to use incremental for G71. The D value that is put in the G71 is incremental radius measure and the U and W for the finish allowance are both incrmental measure but the program block selected by the P and Q can be all absolute. You would set your start X and Z; if Z zero is taken at the end of the stock then these would be X20. Z0.5 to give a little Z clearance. Your feed (F) is .075 and you want to take off 0.5mm per pass so D is .25 so your program would have something like this: Choose tool Start spindle G00 X20. Z0.5 (Move to start position) G71 P3 Q4 D0.25 U0. W0. F0.075 N3 GOO X6.0 Z0.0 N4 G01 Z-40. Rest of program This format is for Haas operating in Fanuc mode, I think some machines require you to put entries on two separate lines but the principle is the same.

A 2-block example:

G00 X20. Z0.5 (Move to start position)
G71U.25R.25
G71 P3 Q4 U0. W0. F0.075
N3 G00 X6.0
N4 G01 Z-40.

Not positive, but I don't think you can have the Z0.0 in Geof's example.

If 6mm diameter x 40mm long is finish size, and you are using another tool to finish with, then you need to give the U0W0 a value. U-value is a diameter value for the 2-block cycle. In the example above, I would eliminate the U & W. Zero is understood.

What machine is this on? What kind of material? What tool is being used to remove the material? That is normally a finishing cut. Are you cutting heat-treated steel in the 60Rc area? Or something like Stellite?

[wevz]

Thanks for the help. It is working good. The material is an exotic material that is part nickle part chrome and titanium. It can be a real bugger to machine but if it was easy everyone would be doing it. I'm using a carbide, wnmg 331 04 04 kf insert. We manufacture internal parts for turbo chargers.

[g-codeguy]

Originally Posted by wevz Thanks for the help. It is working good. The material is an exotic material that is part nickle part chrome and titanium. It can be a real bugger to machine but if it was easy everyone would be doing it. I'm using a carbide, wnmg 331 04 04 kf insert. We manufacture internal parts for turbo chargers.

Glad to hear it is running good for you. Not familiar with that insert, but I am guessing that KF is a finishing chip breaker. I usually prefer a ground insert for cutting tough materials. (In a positive rake tool if I have chatter problems due to small diameters.) The edges aren't as strong as a molded negative tool, but it will do a better job of actually CUTTING the material.

A molded insert in a negative tool taking anything resembling a rough cut in this kind of material usually winds up pushing the material back through the collet on our barfeed machines. Even with collet pressure at maximum. Sounds like you've got a good handle on it.

[wevz]

I am not understanding the change tool final/finish cut with the G71. I am making the final cut with another tool not using the G71. I think there is an easier solution. I am going to try to place the program on here. If anyone can help, it open in wordpad.

%
O4342(724342 PIN SAMPLE)
(G54 Z 170.362)
(O.D. 6.15-6.45 6.3)
(LENGTH 33.68-34.18 33.93)
(NECK DIA. 5.27-5.57 5.42)
N5G21G90G97G99
G54T0317
G0Z100.
N10G50S3000
N15G54T0114(ROUGH O.D.)
N20M04S2500
N25M8
N30G0X10.Z1.(STARTING DIAMETER)
N35G71U.25R.05
N40G71P45Q50U0.W0.F.075
N45G0X6.4Z1.
N50G01Z-37.128
N55G0X6.4Z50.
N60M9
N65M5

M01
N70G54T0515(FINISH O.D./FACE)
N75M04S2500
N80M8
N85G0X6.5
N90Z0.
N95G01X-1.8F.02
N100G0X3.604
N105G03X5.242Z-.667R.9F.02
N110G01X6.3Z-2.64(X=FINAL DIAMETER)
N115Z-37.128
N120G0X6.4Z50.
N125M9
N130M5

M01
N135G54T0316(NECK GROOVE/CUTOFF)
N140M04S850
N145M8
N150G0X6.6
N155Z-6.72
N160G01X5.42F.01
N165Z-11.766
N170X8.3Z-13.369
N175G0Z-34.945
N180G01X5.331Z-35.93F.01
N185X-1.4
N190G0X7.3
N195Z50.
M9
M5

M01
N200G54T0317(STOP BLOCK)
N205G0X-33.4
N210Z.93
M30
%

[g-codeguy]

Not sure I understand your problem with the G71 cycle. It is a roughing cycle only. If you want to incorporate a finishing pass using the blocks defined in the G71 cycle, you will have to use the G70 cycle. This will require you to program the G71 with finish dimensions, and adding values into the U & W so as to leave stock for the finish pass. Finish feedrates will also have to be included. Looking at the samples for G71, G72, & G73 in one of my operator manuals shows the finishing pass (G70) for each canned cycle being completed with the roughing tool in the same operation.

Don't know about you, but I seldom rough & finish with the same tool, & have never used the G70 cycle.

An earlier poster was correct. You can also use a 'Z' in the 1st block of the G71. I tried a Z-value being the same as my starting position, less than starting position, and greater than starting position, & they all ran on a 21i-T control. However, it is unnecessary as long as it is the same as the starting position. I always first position my tool at the correct Z-value.

I would rough turn deeper than the finish turn goes so that the finish insert doesn't run into the stock. I consider block N100 to be a poor machining practice. I never rapid across a finish surface . It often will leave swirl (drag) marks. I wouldn't even use a rapid move for that short a distance. My program would look like this:

G1X-1.8F.02
Z.5F.65
X3.605
Z.15
Z0F.02
G3X5.242Z-.667R.9
ETC.

OR if you prefer to rapid move

G1X-1.8F.02
G0X3.1Z.5
G1X3.605Z.15F.65
Z0F.02
G3X5.242Z-.667R.9
ETC.

These are personal preferences. I don't like rapiding to the final position for this type of action. I would rapid to a Z-value if I was going to semi-finish a shoulder.

I would also use more than .1 clearance for your rapid move at the end of the finish turn operation. Too close. Running heat-treated 675 Pyrowear with a .01 retract move (.255 for you metric blokes) in a G71 cycle caused the tool to put drag marks on the O.D. when it made the rapid move back to the starting position for the next cut. It was springing that bad on 1/2 inch material.

Like you, I programmed with line numbers and G00, G02, M09, etc. when I first started. Now I use line numbers on the 1st block of each operation, & where needed in canned cycles. G00, G03, M09, etc. are now programmed G0, G1, M9, ETC. Takes up less memory, & I got lazy as I got older.

Don't know the machine you are using, so I don't know its format, but M9 in my programs would be on the feed pullout move or (in your example) on the rapid clearance move. Same for the M8. It would be on an approach move. Maybe your M-codes have to be on a separate line. Don't know.

EDIT: For clarification, the above comment about using the G70 cycle means that the G70 is used WITH the G71 cycle. Example for 1.5 inch material, turn .67 diameter with .062R on front & a 45 degree angle starting 1.0 deep & extending to stock O.D. using a .031R insert.

N100G0X8.Z5.M8 (ROUGH/FINISH TURN)
G97S1984M3
T0101
X1.54Z.005
G50S3000
G96S800
G1X.2F.01
X-.065F.004
G0X1.5Z.03
G71U.069R.02
G71P1Q3U.01W.005F.01
N1G0X.46
N2G1X.484Z0F.003
G3X.67Z-.093R.093
G1Z-1.0183F.005
N3X1.5Z-1.4333F.004
G0X.7Z0 (FINISH FACE)
G1X-.065F.004
G0X.47Z.02
G70P2Q3 (FINISH TURN)
G0G97Z1.M9
X8.Z5.T0100
M1

Had this example come from a book block N1 would read X.484 and block N2 would not have an X-value. Hope I explained it clearly enough.

[wevz]

g-codeguy
Well that's quite a bit of enfo to take in. You really have been very helpful. As you can see I am new at programming, it sure makes life easier to have someone to answer questions rather than learning EVERYTHING the hard way! (As in crashing)