G73 & G42 Question

[TimHutchinson]

I am trying to machine the groove in a cast sheave. I am running it on a sharp lathe with Fanuc 18I controller.

Because the sheave is cast, I would like to use the G73 canned cycle to clean it up and do finish cut. I am having problems with the TNRC when I try to loop the program. When I remove the G73 code and just run it with the G42, it appears to work fine.

Here is my code:

G90 G40
T0616
M03 S150

G00 X9.00 Z2.00

G73 U2.25 W0.00 R46
G73 P10 Q50 U0.080 W0.00 F0.015

N10 G00 X7.5 Z2.00
G42 G01 Z1.00
G01 Z-0.146
G03 X7.129 Z-0.387 R0.25
G01 X4.940 Z-0.681
G02 X4.940 Z-2.069 R0.719
G01 X7.129 Z-2.363
G03 X7.500 Z-2.604 R0.25
G01 -3.00
G01 X8.5 Z-3.50
N25 G40 G00 X9.5

M05
M30

Any ideas are appreciated!

Tim Hutchinson

[mark c]

Wow it's been a while since I've done any pattern repeats.
Shouldn't the Q be 25 to match the N25?

[Muzzy]

here is a good web sit.
http://home.columbus.rr.com/hputz/

[TimHutchinson]

Mark,

Yeah. I caught that one but didn't change the file I posted.

Tim

[tobyaxis]

Originally Posted by TimHutchinson I am trying to machine the groove in a cast sheave. I am running it on a sharp lathe with Fanuc 18I controller. Because the sheave is cast, I would like to use the G73 canned cycle to clean it up and do finish cut. I am having problems with the TNRC when I try to loop the program. When I remove the G73 code and just run it with the G42, it appears to work fine. Here is my code: G90 G40 T0616 M03 S150 G00 X9.00 Z2.00 G73 U2.25 W0.00 R46 G73 P10 Q50 U0.080 W0.00 F0.015 N10 G00 X7.5 Z2.00 G42 G01 Z1.00 G01 Z-0.146 G03 X7.129 Z-0.387 R0.25 G01 X4.940 Z-0.681 G02 X4.940 Z-2.069 R0.719 G01 X7.129 Z-2.363 G03 X7.500 Z-2.604 R0.25 G01 -3.00 G01 X8.5 Z-3.50 N25 G40 G00 X9.5 M05 M30 Any ideas are appreciated! Tim Hutchinson

G00 X9.00 Z2.00

G73 U2.25 W0.00 R46<<<<<<<<(W)- How much does this have to clear?
G73 P10 Q25 U0.080 W0.00 F0.015 <<<<<<<(W)- How much material do you want left for finishing?

N10 G00 X7.5 Z2.00
G42 G01 Z1.00
G01 Z-0.146
G03 X7.129 Z-0.387 R0.25
G01 X4.940 Z-0.681
G02 X4.940 Z-2.069 R0.719
G01 X7.129 Z-2.363
G03 X7.500 Z-2.604 R0.25
G01 -3.00
G01 X8.5 Z-3.50
N25 G40 G00 X9.5

M05
M30

I changed the Q50 to Q25 so it will read from P10 (N10) to Q25 (N25).

Also make sure your Offset Geometry is correct with the tool tip designation (0-9) and Radius of the tool tip. Set the tool tip to Tip 3 if this is a CNMG Style Insert and Holder

[TimHutchinson]

Originally Posted by tobyaxis G73 U2.25 W0.00 R46<<<<<<<<(W)- How much does this have to clear? G73 P10 Q25 U0.080 W0.00 F0.015 <<<<<<<(W)- How much material do you want left for finishing?

I want to leave about 0.040 on for finishing. As far as clearance, that is another issue. When I was experimenting, any W value on the first G73 line would offset it one way in the Z direction. Because this part is a groove, offsetting one way would leave metal on one side and take extra metal on the other. (see dxf)

My offsets and tnr seem to be working correctly when not in a G73 cycle.


Tim

[Sump Cleaner]

Tim,

The G73 code will not support TNRC when it is roughing. You will need to program the path on the computer without TNRC and rough it out, then finish it with a G71 with the tool nose comp on or write a seperate chunk of code for finishing.

JK

[TimHutchinson]

Thanks JK,

The G71 will work with the TNRC?

Tim

[Sump Cleaner]

Tim,

You may want to write the seperate chunk of code for the finishing pass. The comp does work sometimes in G71 (sorry, this should read G70 for finishing) with the G71 turning or the G72 facing but it fails for the G73 usually because the code you write to rough it out is rarley the same as the code you need to finish the part.

What tool shape are you using?

JK