Need Help!- G71 is doing square dance at Z1.01

[peelmachining]

Hello I need help with G71.
I Have oi-T controller on a Feeler Lathe.
I am boring from 20mm to 38mm diameter
It is very frustrating and am thinking of programing long hand to get around it for now.

The problem is it feeds up X+ a couple of times as if facing at Z1.01 (W.01) like it is doing a square dance, then goes to cut the finish diameter at 38mm (with a 20mm initial bore that is 14mm depth of cut).

This is the code, I am not using G70 finishing.
G00 X20. Z1.
G71 U2.5 R.3
G71 P300 Q400 U-.2 W.01 F.2
N300 G00 X38. Z1.
G01 X38. Z-58. F.15
N400 G00 X35. Z1.
G00 Z30.

Any ideas Please
Thanks in advance for your help.


Regards
John

[fordav11]

what you're doing is very simple in programming terms.

As a general rule the start point in X (before the G71) and the end point on the last N line (the line number denoted by Q) should be the same X value. Looks like the end X35. is messing it up.

I would write it like this.....

G00 X20. Z1.
G71 U2.5 R.3
G71 P300 Q400 U-.2 W.1 F.2
N300 G00 X38.
G01 Z-58. F.15
N400 X20.
G00 Z30.

There's no need to put a G00 and Z on the N400 line either. The machine will automatically return the tool to the start point after it finishes the roughing cycle. so after N400 it would move to X20. Z1. by itself then Z30.0

note that the F.15 does nothing here. The roughing feed is taken from the G71 line. If you were to use G70 P300 Q400 then F.15 is used.

I would also put a bit more on W or you'll see steps on the back face which won't be cleaned up by a finish tool, unless the finish tool is going deeper than Z-58.0

In any case the depth of cut the machine takes will be 2.5mm. If this does not work maybe your machine has other issues?

[peelmachining]

There's no need to put a G00 and Z on the N400 line either. The machine will automatically return the tool to the start point after it finishes the roughing cycle. so after N400 it would move to X20. Z1. by itself then Z30.0

I did this yesterday ( leave out the Z) I then did a test no material with a restart at G70
well that boring bar is no more because it stopped at the back of the bore rapid to X35. the next line after G70 P Q read
G00 X250. Z 20.
so it rapid there through the jaws and smashed to bits I would have been fine if i had not taken this advice and taken out my safety Z

I will try your other sugestion
Regards
John

[fordav11]

heheh. Not funny I know but still funny
Ouch!
Well there's a parameter not set right. It should come out by itself.
Let me look it up.....
Hmm, well I'm sure there was something in the parameter manual about that but I don't see it now. Maybe there is no parameter setting for that. It just comes out back to the start by itself.
A G70 is a different story. It follows the path from N300 to N400.
after the G70 you should always put G00 Z1.0 or some other clearance Z value.

technically you should be finishing with a different tool, so the complete program should look something like.....

N1 G50 S1000
G0 T0101
G96 S150 M3
G0 X20. Z1. M8
G71 U2.5 R.3
G71 P10 Q11 U-.2 W.1 F.2
N10 G00 X38.
G1 Z-58. F.15
N11 X20.
G0 Z1. (optional)
G0 X300.0 Z200.0 M9
T0100
M1
N2 G50 S1000
G0 T0202
G96 S200 M3
G0 X20. Z1. M8
G70 P10 Q11
G0 Z1. (NOT optional)
G0 X300.0 Z200.0 M9
T0200 M5
M1
M30

I like to keep each tool with a unique N number per operation.
So 1st tool uses N1 and any cycle uses N10 to N11 then N12 to N13 then N14 to N15 etc.
For 2nd tool, N2 then any cycle there uses N20 to N21, N22 to N23 etc. Keeps it nice and simple and makes searching though the program easy. To restart the finish cut just leave it in memory, type 2, press N-SEARCH then press start


hehe. I'm still grinning about your bar, cant help myself. I've seen people put a 50mm or 60mm devibe boring bar (costing $5k) that was 400mm or 500mm down a bore through the side of a job at high speed. All sorts of bad damage done and a nasty sound it makes too. That machine was repaired but its still not 100% right

[peelmachining]

ok making line N400 X20. Z1.
has made the dance different ????
it now cuts 14mm deep in Z
comes out adds a cut in X then cuts to 25ish in Z
then out and another cut in X to 38ish deep Z

turning the machine of then on does nothing????

I have tried about 50 different combinations getting really bumbed about it.
the Fanuc book has no exceptoinal explanations either.

[fordav11]

hmmm very strange. it looks like its trying to rough a taper?
The G71 is right, you dont really want to use the other more simple but longer to program roughing cycles. I've been programming for 25 years and never used them once

As for your problem, I'm not sure what's going on.
What happens after the last cut at Z-38.?
And what are the X cuts at each Z value you listed?

It should move like this....
G0 X20.0 Z1.0
X19.6 Z1.1 (reads G71 U- W+)
G0 X24.6
G1 Z-57.9 F0.2
X24.0 (this is the R value working, -0.3 in X on radius back-off for each cut)
(some machines would take the cut to X19.6 then an extra movement X19.0 Z-57.3 depending on parameters and model)
G0 Z1.1
X29.6
G1 Z-57.9
X29.0
G0 Z1.1
X34.6
G1 Z-57.9
X34.0
G0 Z1.1
X37.8
G1 Z-57.9
X19.8
G0 Z1.0
G0 X300.0 Z200.0
or something like that etc


In a G71 the last pass should take a cut of the full profile to clean up any steps made by the roughing cuts leaving the finishing allowance on.
Does your machine do that?

If not I think your machine has other issues.
Maybe program it long hand for now until you figure it out or can get someone to look at the machine.
Actually try doing it long hand anyway (copy paste my program above)
If that works then your machine is probably ok but some parameters are not right. maybe ;-)

[sinha_nsit]

Without a drawing examining a code in not enjoyable.

[fordav11]

if you need a drawing to figure out a simple straight rough boring cycle then you probably need to look for an easier job

[g-codeguy]

forday has given you spot on advice. I am not aware of any canned cycle that doesn't end at the same place as the starting point. The line with the second X20. isn't needed unless you want to face a shoulder. I rough turn and rough bore past the cut-off point all the time without such a block as I'm not concerned about a smooth face at these points.

In such a situation, my program would look like like this:

G0 X20. Z1.
G71 U2.5 R.3
G71 P300 Q400 U-.2 W.1 F.2
N300 G1 X38.
N400 Z-58.
G00 Z30.

provided I ever were to program in metric.

I quit using a G0 in the G71 many years ago because I no longer believe in rapid moves for such a short distance.

I know sinha_nsit is a smart young man, but I can understand forday's comment if he isn't familiar with sinha_nsit's posts. Maybe sinha_nsit didn't read the OP's post very closely. Even a beginning programmer could read that code and understand what it was doing!

[sinha_nsit]

Originally Posted by g-codeguy ...Maybe sinha_nsit didn't read the OP's post very closely. Even a beginning programmer could read that code and understand what it was doing!

Exactly.
Actually, without reading the post carefully, I assumed that the profile might be a complex one. After all, why not use a simpler G90 for straight turning which involves only a few passes.

Incidently, I am not in a CNC-related job. It is just my hobby. I do not make a penny out of it.

[dcoupar]

Originally Posted by sinha_nsit Exactly. Actually, without reading the post carefully, I assumed that the profile might be a complex one. After all, why not use a simpler G90 for straight turning which involves only a few passes. Incidently, I am not in a CNC-related job. It is just my hobby. I do not make a penny out of it.

G90 feeds the tool back to starting X (in this case 20mm) at the end of each pass. This is a waste of time and not especially good for the insert.

[sinha_nsit]

That is right, if a lot of material is to be removed.
We can, however, make it more efficient by changing the start X after. say, every five passes.