[JWB_Machining]

Hey,

I'm turning down a reduced diameter on a bar. My roughing cycle goes fine. When it's done it oddly retreats to a start point 0.020" closer to my tail stock then I expect it to and then makes a tiny cut in and starts the finishing pass. I want to get rid of this tiny vut in but for the life of me I can't figure out what's causing it which means it's probably cutter comp or sometihng like that. I could just get rid of the finishing pass all together but I feel like that's letting the machine defeat me. I'm using a TL-1, below is the code:

O00056
G18 G40 G64 G80 G97 G99
M09
T606 (T)
G97 S500 M03
G54 G00 X0.535 Z-2.25 M08
G96 S300
G71 P101 Q102 U0.003 W0.002 D0.01 F0.006
N101 G00 X0.532 Z-2.25
G01 G42 D3 X0.528
G02 X0.2494 Z-2.3847 R0.187
G01 X0.2497 Z-3.0625
X0.2514 Z-3.7403
G02 X0.53 Z-3.875 R0.187
G01 X0.53
N102 G40 X0.55
G70 P101 Q102 F0.002
M09
G00 X4. Z0 M09
M30

[txcncman]

I disagree with your lead-in and lead-out moves. What is the nose radius of the tool?

Try something like this:

O00056
G18 G40 G64 G80 G97 G99
M09
T606 (T)
G97 S500 M03
G54 G00 X0.55 Z-2.2 M08 <changed
G96 S300
G71 P101 Q102 U0.003 W0.002 D0.01 F0.006
N101 G01 G42 D3 X0.528 Z-2.25 <changed
G02 X0.2494 Z-2.3847 R0.187
G01 X0.2497 Z-3.0625
X0.2514 Z-3.7403
G02 X0.53 Z-3.875 R0.187
G01 X0.53
N102 G40 X0.55 Z-3.9 <changed
G70 P101 Q102 F0.002
M09
G00 X4. Z0 M09
M30

[JWB_Machining]

The Tool Radius is 0.0312

I'm going to try the program you gave me in a little bit. I'll let you know how it goes this afternoon. Thank you.

What was the logic behind the changes the lead in and lead out? Most of my work comprises running programs similar to this and I'd like to have a better understanding of what's going on. I thought I understood G02 Commands but when I'm not turning a 90 degree radius I get confused, ie if the radius I want is .250" but the change in diam is less than that. I've had issues where instead of getting, for lack of better terms, a paranthesis I get a smile. Haha that sounds ridiculous. I can upload a sketch later if you need.

Thanks again.

[txcncman]

The practice for years as applies to older controls is that the lead-in and lead-out moves must equal or be greater than the radius of the tool (as input in the tool table). I do not know if this was the actual problem, but potentially if could have been. Also having the ending X being larger than the start point X would cause the tool to drop the the start point X while returning to the start point Z at the end of the cycle. For your part, I do not think this would have crashed, but I could give an example where it would crash into the part if you would like.

[JWB_Machining]

Hey,

Still no luck. I put up the graphics images generated on my machine. 0503 is your program, 0504 is the one I posted.

[KenFoulks]

As stated previously, cutter compensation logic dictates the lead-in/out must be greater than the radius of the tool.


Change these three:

G54 G00 X0.55 Z-2.2 M08
N101 G01 G42 D6 X0.528 Z-2.25
N102 G40 X0.562 Z-3.9

[txcncman]

I think you are seeing the results of 2 things happening. One is in the System Settings and has to do with the amount the tool backs off the cutting in both X and Z during roughing cycles. The other is the W in the roughing cycle itself, the amount to leave for finishing.

You might consider switching to G73 cycle for this and leave W at 0.000.

The alternative is to write your own tool movements for each roughing pass.

[KenFoulks]

I think you are seeing the results of 2 things happening. One is in the System Settings and has to do with the amount the tool backs off the cutting in both X and Z during roughing cycles..

Excellent point, setting 73 controls the canned cycle retraction. Reduce this value and you should be able to see the difference.