Need Help!- WRONGLY MENTIONED END POINT IN G71 canned cycle

[DEVENDRA]

i have wrongly mentioned the end point in the rough turning canned cycle, 'i like to know what will happen, when the below program is excuted,

G72 w0.5 r0.5;
G72 p10 q20 u0.0 w0.0 f0.18;
n10 g0 z0;
g1 x-1;
N20 G0 Z1.0;
G0 X17.0 Z1.0;
G71 U1.5 R0.5;
G71 P30 Q40 U0.2 W0.1 F0.18;
N30 G0 X5.20;
-------
-------
N20 G1 X18.00;
G0 X19.00 Z1.0;
T0;
G0 X0.0 X-150.0;

[sinha_nsit]

G72 is not correct.

In G71, the last point on the profile lies above the initial tool position(X18 vs X17).
Roughing would be done starting from X17, but the tool would go up to X18 in the step-removal pass of G71. Finally, the tool would come back to X17 at the end of the cycle, showing dog-leg effect. This technique is useful for repeating G71 on a previous partial machining with G71 (which got aborted due to reasons like power failure). You can skip unnecessary roughing passes. But, you need to be careful about dog-leg effect; the tool may have interference with job during retraction.

[g-codeguy]

The G71 cycle won't run. It will alarm telling you it can't find the missing number. Unless you have an N40 block some where else in the program. Then what is does would depend on what is in the program between blocks N30 and N40.

EDIT: In the G72 put block N20 on line g1 x-1; The block before the G72 call is the starting position for the canned cycle. X should be a clearance point. Z should be the point where the material to be removed starts at.

So if you were running 17mm stock with 5mm that needed to be faced off, your starting point should be

X18.Z5.

Normally you wouldn't program an X ending point larger than the X starting point as the starting point should be the same diameter as the material being removed. Why would you want to cut air? As for sinb_nsit's suggestion about skipping unnecessary roughing passes for something like a power failure, I wouldn't be changing my program for one part unless it was way way bigger than anything I've ever run before. How much time are you going to lose rerunning the cycle on one part?

[sinha_nsit]

There is no harm in keeping the end point slightly higher than the start point. Roughing starts from start point only; there would be no air-cutting. The only difference would be in the step-removal pass of G71 (I am referring to type I cycle) where the tool would go up to the specified end point. In fact, this might give a better corner. Cycle time would remain nearly same.

Yes. There is no point in modifying the program for just one job. In fact, modification may take more time than it would save. I was talking about only a theoretical possibility.

I read N20 as N40!

[g-codeguy]

Originally Posted by sinha_nsit There is no harm in keeping the end point slightly higher than the start point. Roughing starts from start point only; there would be no air-cutting. The only difference would be in the step-removal pass of G71 (I am referring to type I cycle) where the tool would go up to the specified end point. In fact, this might give a better corner. Cycle time would remain nearly same. Yes. There is no point in modifying the program for just one job. In fact, modification may take more time than it would save. I was talking about only a theoretical possibility. I read N20 as N40!

How would having a larger end point than start point result in a better corner (I assume we're talking about stock OD corner) since the cutting edge of the tool would be a full insert radius above the material? Unless there is a humongous burr there from roughing. I admit to facing an approximate .05 (inches and from the center line of the insert radius, not the front) below a drilled hole so there isn't any material sticking out in front of the face when my boring bar comes in. Of course I could start the bar further away, but most of my jobs are small parts so it is faster to face the extra distance since I also kick the feedrate up once the insert radius is a few thousandths past the hole.

Well...I guess I've answered my own question!

[sinha_nsit]

You are right.
Might also means might not!
Actually, I did not give it a very serious thought.

[tanvon]

Originally Posted by sinha_nsit G72 is not correct. In G71, the last point on the profile lies above the initial tool position(X18 vs X17). Roughing would be done starting from X17, but the tool would go up to X18 in the step-removal pass of G71. Finally, the tool would come back to X17 at the end of the cycle, showing dog-leg effect. This technique is useful for repeating G71 on a previous partial machining with G71 (which got aborted due to reasons like power failure). You can skip unnecessary roughing passes. But, you need to be careful about dog-leg effect; the tool may have interference with job during retraction.

Hi
the dog-leg effect is really must to check it might break your tool because tool comes with G00.