TL-1 and G71 Canned Cycle Issue

I can't figure out what I'm doing wrong on this piece of code for my manufacturing class, I think I'm forcing the roughing canned cycle to be a Type II but I'm still getting alarm codes for non-monotone. Any help would be greatly appreciated.

%
O0001
(PROGRAM NAME - CNC LATHE LAB)
(DATE - 24-01-17)
(MATERIAL - ALUMINUM 1.5 IN - 6061-T6)


N10 G20 G99
N20 T0101
N30 G50 S2000
N40 G96 S250 M03
N50 G00 G54 Z0.1
N60 X1.6


N70 G71 P80 Q180 U0.01 W0.005 D0.05 F0.008
N80 G01 X-0.05 Z0.1 F0.005
N90 Z0.0
N100 G03 X1.0 Z-1.0 R0.65
N110 G02 X0.9 Z-2.0 R1.15
N120 G01 W-0.1
N130 U0.1
N140 W-0.1
N150 U0.1
N160 Z-2.5
N170 X1.45 Z-3.0
N180 G00 X1.6 Z0.1
N190 G80
N200 M05
N210 M01


N220 T0202
N230 G50 S2000
N240 G96 S350 M03
N250 G00 G54 Z0.1
N260 X1.6
N270 G70 P80 Q180
N280 G80
N290 M05
N300 M30
%

Try removing the Z0.1 from N180. Also I wouldn't put a G00 in that block, as it will rapid up from 1.45 to 1.6. The cycle will return to the start point at G00 automatically.

N180 X1.6

I'm still getting a non-monotone error in my simulator (I'm using GWizard) but I'll run it on the graphics display on my Haas controller to test it out.

That makes sense about the rapid, thank you. Is the start point considered the position just before the G71 command, or the first line of code within the G71 block?

Looking deeper, I'm confused at the X and Z valuies in the 1st couple of blocks of the shape definition. Can you post a drawing of the part please?

The start point is the position just prior to the G71 block.

Attachment 351938

I have the N80 block at X-0.05 because I was hoping to get rid of the little tit at the start of the ball due to the nose radius of the tool.

A couple of thoughts/suggestions:

You're not using G42 to compensate for the tip nose radius, so if you were to cut this part, it wouldn't look like the print (unless you have a sharp tool).

You should dimension your part print to 4 decimal places. If the start-point, end point, and radius don't add up, the control can do some weird things when interpolating arcs.

I believe your U0.1 moves in N130 and N150 should be U0.2.

Dave

I had asked the machinist about running G42, he was telling me that I don't need to worry about this because the tool offset will account for it after turning down a section and measuring the diameter and entering that into the controller. Is that correct? Initially, I thought I needed to run a G42 command.

My apologies for the drawing, it was just a screenshot of my revolve sketch from SolidWorks. However, all of those dimensions do not have any further decimals. I think the U0.1 are correct, all of the step elements are 0.100" in width or radial height.

*EDIT* Or is the U0.1 a diameter movement, so it would actually only move 0.05 in the radius?

The tool offset only adjusts for the X and Z position of the virtual tip, but unless you use G41/G42, you'll need to compute the tip nose radius adjustment for each arc and angled line, and this is laborious if you're not fluent at trig.

Yes, U0.1 is a diameter command, so the actual move amount will be 0.05.

The coordinates of the workpiece contour points given enough accurate.
It is necessary to specify the coordinates of the points to the fourth decimal place.

N50 G54
N60 G00 X1.6 Z0.1

N70 G71 P80 Q180 U0.05 W0.01 D0.05 F0.008
N80 G1 X0 Z0.1
G1 G42 Z0
G3 X1. Z-1.0653 R0.65

G1 X1.6
N180 G40 G1 X1.7

These are the dimensions to the 4th decimal place:
Attachment 351962

Updated code per everyone's suggestions, except the nose radius comp. I'm not so concerned at getting the exact profile right now, I just need to have the code to run hah. I'm still getting the same alarm code.

%
O0001
(PROGRAM NAME - CNC LATHE LAB)
(DATE - 24-01-17)
(MATERIAL - ALUMINUM 1.5 IN - 6061-T6)

N10 G20 G99
N20 T0101
N30 G50 S2000
N40 G96 S250 M03
N50 G54
N60 G00 X1.6 Z0.1

N70 G71 P80 Q180 U0.05 W0.01 D0.05 F0.008
N80 G01 X0. Z0.1 F0.005
N90 Z0.
N100 G03 X1.0 Z-1.0 R0.65
N110 G02 X0.9 Z-2.0 R1.15
N120 G01 W-0.1
N130 U0.2
N140 W-0.1
N150 U0.2
N160 Z-2.5
N170 X1.45 Z-3.0
N180 X1.6
N190 G80
N200 M05
N210 M01

N220 T0202
N230 G50 S2000
N240 G96 S350 M03
N250 G00 G54 Z0.1
N260 X1.6
N270 G70 P80 Q180
N280 G80
N290 M05
N300 M30
%

To test, try this code

N10 G20 G99
N20 T0101
N30 G50 S2000
N40 G96 S250 M03
N50 G54
N60 G00 X1.6 Z0.1
N70 G71 P80 Q180 U0.05 W0.01 D0.05 F0.008
N80 G01 X0. Z0.1 F0.005
G1 Z0.
G3 X1 Z-1.0653 I0 K-0.65
G2 X0.9 Z-2. I0.6031 K-0.5009
G1 Z-2.1
G1 X1.1
G1 Z-2.2
G1 X1.3
G1 Z-2.5
G1 X1.45 Z-3.
N180 X1.6
G0 X2. Z2.
M05
M01

I have to ask this, as I don't see anything that should cause the alarm: Are you manually typing in your program here, or downloading it from the machine and copying the program to your post. I've seen so may instances where there's a typo in the post, and what we see isn't exactly what's in the control.

Just some random thoughts on your last posted code:

N80 G01 should probably be G00.

N90 should be G01 Z0 F0.005

I believe N170 X1.45 should be X1.48.

I don't see any move away from the part before indexing to T0202. The Haas manual shows G53 X0 and G53 Z0 before an index and at the end of the program.

One more thing: Please check Setting 33. If it's set to YASNAC, then you'll need to add R1 (with no decimal) to N70 to activate type II roughing.

Thanks for all of the help. I will check the latest code on the Haas controller on Monday. I'm loading the file in from my USB stick which I have copy and pasted from the forums here, so there shouldn't be any typos that aren't apparent on here.

That looks like a pawn for a chess set.

Anyway, I had a similar problem early last year when making a chess set. What I did in the end was draw the profile in autocad and import that into the graphics of the TL-1 and have it generate the code automatically. Took me a few tries to get it right, but in the end it made a very nice show piece for out display case.

For the import, just put the profile on a USB 2.0 thumb-drive, and select the drawing like you would any other program. Also, the 0,0 position of the part must be at 0,0 of what ever cad program you use to generate it. From there it will make the code for you. The tricky bit is getting the U and W values sorted as that is where the thing gets confused when generating the program. Just check the program in edit and cut a test piece out of some sort of soft stock, preferably plastic of some sort.

Here's a link for the similar problem I was having, with pics and code, Profile drawn with auto-cad and code generated auto-magically by the TL-1. Never did get that issue sorted out. :(

http://www.cnczone.com/forums/haas-l...ile-issue.html

Quote:

---

Originally Posted by kstopp

Thanks for all of the help. I will check the latest code on the Haas controller on Monday. I'm loading the file in from my USB stick which I have copy and pasted from the forums here, so there shouldn't be any typos that aren't apparent on here.

---

This code works well.

%
O75007
N10 G20 G99
N20 T101
N30 G50 S2000
N40 G96 S250 M03
N50 G00 G54 Z0.1
N60 X1.6


N70 G71 P80 Q180 U0.01 W0.005 D0.05 F0.008
N80 G01 X-0.05 Z0.1 F0.005
N90 G42 Z0.
N100 G03 X1. Z-1. R0.65
N110 G02 X0.9 Z-2. R1.15
G01 W-0.1
N130 U0.1
W-0.1
N150 U0.1
N160 Z-2.5
N170 X1.45 Z-3.
G01 X1.6
N180 G01 G40 X1.65
N190 G80
N200 M05
N210 M01


N220 T202
N230 G50 S2000
N240 G96 S350 M03
N250 G00 G54 Z0.1
N260 X1.6
N270 G70 P80 Q180
N280 G80
N290 M05
N300 M30
%

Hello, DMCain,
Here is the working code for chess king with the G71.

%
O75006
(CHESS KING)
(END FACE)
G20
T202
G54
G50 S2000 M08
G96 S850 M03
G00 X1.1 Z0.075
G72 P10 Q15 U0 W0 D0.01 F0.005
N10 G00 Z0.
G01 X-0.05
N15 G01 X-0.05 Z0.05
G00 X1.2 Z0.
M01


(PROFILE)
T202
G54
G50 S2000 M08
G96 S850 M03
G00 X1.1 Z0.05
G71 P20 Q25 D0.01 U0.01 W0.008 F0.008
N20 G01 X0. Z0.05
G01 Z0.
G01 X0.125
G01 X0.1248 Z-0.0749
G01 X0.275
G01 Z-0.1499
G01 X0.1248 Z-0.2386
G01 Z-0.2682
G03 X0.2498 Z-0.3809 R0.125
G03 X0.7498 Z-0.4297 R1.3125
G01 Z-0.46
G00 X1.1
N25 X1.2

G70 P20 Q25

G00 X1.1 Z-0.38

G71 P30 Q35 D0.01 U0.01 W0.008 F0.008
N30 G01 X0.7498 Z-0.38
Z-0.4297
G02 X0.6212 Z-0.7921 R1.0527
G01 X0.6212 Z-0.8558
G02 X0.3654 Z-1.0938 R0.2854
G02 X0.5 Z-1.2778 R0.2854
G01 Z-1.3416
G02 X0.9664 Z-2.7948 R1.3227
G03 X0.9998 Z-2.8373 R0.0625
G01 Z-2.9
G01 X1.1
N35 G01 G40 X2.45
G70 P30 Q35
G00 X2.5 Z6.
M30
%

Thanks for the help everyone, my code ran perfect today. I think it may have been my initial N180 line that was causing an issue. This was the final code:

%
O0051
(PROGRAM NAME - CNC LATHE LAB)
(DATE - 24-01-17)
(MATERIAL - ALUMINUM 1.5 IN - 6061-T6)

N10 G20 G99
N20 T0101
N30 G50 S2000
N40 G96 S250 M03
N50 G54
N60 G00 X1.6 Z0.1
N70 G71 P80 Q180 U0.02 W0.01 D0.05 F0.008
N80 G00 X0. Z0.1
N90 G01 Z0. F0.005
N100 G03 X1.0 Z-1.0 R0.65
N110 G02 X0.9 Z-2.0 R1.15
N120 G01 W-0.1
N130 U0.2
N140 W-0.1
N150 U0.2
N160 Z-2.5
N170 X1.45 Z-3.0
N180 X1.5
N190 G80
N200 M05
N210 M01

N220 T0202
N230 G50 S2000
N240 G96 S350 M03
N250 G00 G54 Z0.1
N260 X1.6
N270 G70 P80 Q180
N280 G80
N290 M05
N300 M30
%

http://www.cnczone.com/forums/attach...d=352996&stc=1

I believe your issue was the G01 you had after your G71 start command. I believe the machine thought this was a huge undercut

That was your G01 X0 Z.1
You now have this as a G00 now which is most likely why it worked. I use canned cycles all the time with undercuts and had to overcome all the errors you can think of. ????

Attachment 508795