NEWB with some G71 cycle issues...... HELP!

[pacificcalls]

Hey all!
First post as I am new to the forum and machine world!
Trying to do this on a Haas sl-10 we just picked up and we've hit a HARD snag trying to run our g71 cycle-

I've attempted to do my homework, and understand the basics as far as type I and type II roughing (which this would qualify as type II I believe) but we are just not getting anywhere no matter how basic or complex we attempt to make it--We are continually getting a "non monotonous" alarm.

here is our basic program set up, its cutting the first side on a duck call, ill skip down to a few lines before our g71 and a few lines after--

X1.8 Z.01;
G1 X-.06 F.004;
G0 X1.54 Z.03;
G71 P10 Q11 D.065 U.020 W.005 F.006;
N10 G0 X1.0;
G1 Z0;
X1.134 ,C .0250;
Z- .515;
X1.25 ,C .0250;
Z-.884;
G2 X1.35 Z-1.336 R1.152;
G1 Z-1.5;
X1.54;
N11 G0 X1.54;
G28 M09;
M01;


Thanks in advance for any input, we've tried removing the g2 cycle and making it a straight line, and removing the automatic chamfering to see if it would do it, but cannot break the non monotonous alarm

 

[bigjon61]

Haven't programmed using G71 in a while, but perhaps that rapid move N11 could be screwing things up. Change your N11 to the line before (X1.54). It wouldn't make sense to be "roughing" a rapid move.

Edit: Quick google search yielded the rapid move before the G71 has to be greater (x axis) than the largest diameter in the G71 cycle. Change that to say 1.6 and you should be good to go.

 

[pacificcalls]

Haven't programmed using G71 in a while, but perhaps that rapid move N11 could be screwing things up. Change your N11 to the line before (X1.54). It wouldn't make sense to be "roughing" a rapid move.

Edit: Quick google search yielded the rapid move before the G71 has to be greater (x axis) than the largest diameter in the G71 cycle. Change that to say 1.6 and you should be good to go.

Awesome,
Appreciate the help!, will give those edits a try first thing!

 

[srp61]

If its saying non monotonous its likely your machine doesnt support type 2. Also the last line of the finished shape program(n11) sets your stock diameter for roughing.

You dont need to have your initial positon greater than your stock(in x and z) but its a good idea as the tool can rapid through the workpiece at the end of the cycle.

 

[pacificcalls]

Its a 2007 Which im sure model year has -0- to do with it but i pretty sure it does support it
we run a similar program for another part and it runs no issues--
its set up in a very similar way:

Again type II as I am moving my X

G0 X1.04 Z.03
G71 P10 Q11 D.0650 U.020 W.0050 F.006
N10 G0 X.5
G1 Z0
X.622 ,C.0200
Z-2.0
X.7365 Z-2.5
X1.04
N11 G0 X1.04
G28 M09

This does another piece for us and runs without a hitch each time, unsure as it has the rapids in same spots and diameter values set equal as well.

 

[srp61]

That one works because your x moves in one direction(+). And is therefore monotonous. Your otger example is non monotonus as you have positive and negative x direction moves

 

[pacificcalls]

That one works because your x moves in one direction(+). And is therefore monotonous. Your othger example is non monotonus as you have positive and negative x direction moves

Where is my (-) x move?
if Im following right, I rapid down to x1. then 1.134, then 1.25 then 1.35 then out at 1.54..... which would all be in a (+) direction or am I missing something?

 

[srp61]

Are you sure your g2 is right you have a radius of 1.152 which creates an slight undercut in your profile

 

[sinha]

Are you sure if type 2 is available on your machine?

Check if inserting W0 in the N10 block helps.

 

[angelw]

X1.8 Z.01;
G1 X-.06 F.004;
G0 X1.54 Z.03;
G71 P10 Q11 D.065 U.020 W.005 F.006;
N10 G0 X1.0;
G1 Z0;
X1.134 ,C .0250;
Z- .515;
X1.25 ,C .0250;
Z-.884;
G2 X1.35 Z-1.336 R1.152;
G1 Z-1.5;
X1.54;
N11 G0 X1.54;
G28 M09;
M01;

Hi pacificcalls,
You're getting the "non monotonous" alarm because I believe your use of the DIRECT DRAWING ",C" function is creating a "non monotonous" move in the part profile, but you have only initiated G71 Type I cycle. To make Type II cycle active, an X and Z move in the "P" referenced block is required. By only specifying an X address only, Type I G71 cycle will be active.

Post a sketch of the part shape you want to create.

Specify one of the following two blocks to activate G71 Type II multi-repetative cycle:

1. N10 G0 X1.0 Z.03 (the same absolute Z coordinate as the Z position prior to the G71 cycle being launched)
or, as Sinha suggests,
2. N10 G0 X1.0 W0.0 (a Z incremental move of Zero)

Either of the above block will result in no move in Z when the tool moves to each successive depth of cut, and will activate G71 Type II cycle.

Regards,

Bill

 

[drewboyer]

Why put the G0 in N11? You're already at that point from the last feed move, just make that N11. I only put a rapid in the first line for G71. It goes right back to the starting point as soon as it finishes the cycle.

 

[sinha]

Yes. N11 should be G01, up to just beyond od. Retraction to start point is always rapid, with dogleg effect.
I believe od is 1.5.

 

[pacificcalls]

Hi pacificcalls,
You're getting the "non monotonous" alarm because I believe your use of the DIRECT DRAWING ",C" function is creating a "non monotonous" move in the part profile, but you have only initiated G71 Type I cycle. To make Type II cycle active, an X and Z move in the "P" referenced block is required. By only specifying an X address only, Type I G71 cycle will be active.

Post a sketch of the part shape you want to create.

Specify one of the following two blocks to activate G71 Type II multi-repetative cycle:

1. N10 G0 X1.0 Z.03 (the same absolute Z coordinate as the Z position prior to the G71 cycle being launched)
or, as Sinha suggests,
2. N10 G0 X1.0 W0.0 (a Z incremental move of Zero)

Either of the above block will result in no move in Z when the tool moves to each successive depth of cut, and will activate G71 Type II cycle.

Regards,

Bill

Bill,
Thanks for the reply! ill get to posting a pic here later today, I'll see if adding the z.03 or w0.0 to N10 will get through it (hopefully) if not then i'll start attacking the ",C" functions -

if it does not chew through the ,c then what should I use to chamfer those 90 degree corners? K, program the path manually?

 

[pacificcalls]

Are you sure if type 2 is available on your machine?

Check if inserting W0 in the N10 block helps.

Will do Thanks!

 

[300sniper]

Its a 2007 Which im sure model year has -0- to do with it but i pretty sure it does support it
we run a similar program for another part and it runs no issues--
its set up in a very similar way:

Again type II as I am moving my X

G0 X1.04 Z.03
G71 P10 Q11 D.0650 U.020 W.0050 F.006
N10 G0 X.5
G1 Z0
X.622 ,C.0200
Z-2.0
X.7365 Z-2.5
X1.04
N11 G0 X1.04
G28 M09

This does another piece for us and runs without a hitch each time, unsure as it has the rapids in same spots and diameter values set equal as well.

I'm 99% positive my Fanuc woukd alarm with the redundant X1.04 before the N11. I would get rid of the first one and the G0 in the N11. Maybe Haas doesn't care but it doesn't need to be there.

 

[sinha]

Yes, G00 is redundant but may not cause alarm.

 

[angelw]

if it does not chew through the ,c then what should I use to chamfer those 90 degree corners? K, program the path manually?

Hello pacificcalls,

Following is the part shape as described by your original program; assuming a 0.025 chamfer on the first two corners.



The program below uses auto corner chamfering with "K". The problem I have with using a chamfer to break a corner, is that you end up with two burs instead of one. Even when cutting a small chamfer, of say 0.5mm, I program a very small radius in each corner created by the chamfer so the tool rolls around the corners and you end up with no sharp corners.

Also, as Tool Radius Comp is not being used, and assuming a 1/32" Insert Radius, your 0.025 programmed chamfer would present as an actual chamfer of only 0.0068", or 0.0156 if a 1/64" Insert Radius is used.

Regards,

Bill

X1.8 Z.01;
G1 X-.06 F.004;
G0 X1.54 Z.03;
G71 P10 Q11 D.065 U.020 W.005 F.006;
N10 G0 X1.0;
G1 Z0;
X1.134 K–0.025;
Z- .515;
X1.25 K–0.025;
Z-.884;
G2 X1.35 Z-1.336 R1.152;
G1 Z-1.5;
N11 X1.54;
G28 M09;
M01;

 

[pacificcalls]

Was able to get her rolling last night!

Adding the x and z into the p-block was the ticket!

I did have to remove the ,c as well and replace with k values, but it is spinning!

Thanks for the help everyone!

 

[angelw]

Was able to get her rolling last night!

Adding the x and z into the p-block was the ticket!

I did have to remove the ,c as well and replace with k values, but it is spinning!

Thanks for the help everyone!

Hi pacificcalls,
As stated in my Post #10, the ",C" was creating a non monotonous move in the profile description, and therefore, an X and Z address specified in the P referenced block to activate G71 Type II cycle is required. With ",C" replaced with "K-", there is no longer any non monotonous move in your profile, and therefore, G71 Type I cycle will work with the program shown in my Post #17.

Regards,

Bill