Retract moves in lathe

[Thee Dragracer1951]

I've just crashed my lathe for the second time because of Mastercam. All of a sudden it's not putting in retract moves.

I have not changes a thing. Same post. Same machine def.....

The ONLY good thing about this is that it was in aluminum.

 

Here's the code it posted.

 

 

%

O00000 (69-35800-4)

(DATE - 02-08-08-08:17)

(PROGRAMMED FOR HAAS LATHE)

( T1 OD ROUGH RIGHT - 80 DEG. )

( T3 OD FINISH RIGHT - 35 DEG. )

( T11 CENTER DRILL- .25 DIA. )

( T9 9/32 DRILL )

( T6 OD GROOVE LEFT - NARROW )

(T1 OFFSET - 1)

(OD ROUGH RIGHT - 80 DEG. INSERT - CNMG-432)

G20

G00 T101

G00 X1.2 Z.03

M00

G00 X1.7 Z.1

M31

G97 S1123 M03

G41 G00 G54 X1.7 Z0.005 M8

G50 S3600

G96 S500

G99

G01 X-0.0625 F0.005

G00 Z0.105

G54 X1.4217 Z0.105

G42

Z0.215

G01 Z0.115

Z-0.21

X1.45

G03 X1.47 Z-0.22 R0.01

G01 Z-0.45

X1.5

G40 X1.6414 Z-0.3793

G00 G42 Z0.215

X1.2808

G01 Z0.115

Z-0.21

X1.4417

G40 X1.5831 Z-0.1393

G00 G42 Z0.215

X1.14

G01 Z0.115

Z0.005

Z0.0041

X1.1941 Z-0.0229

G03 X1.2 Z-0.03 R0.01

G01 Z-0.21

X1.3008

G40 X1.4423 Z-0.1393

M9 (No retract move)

G00 G28 X0.0 (BANG)

G28 Z0.0

M01

 

(T3 OFFSET - 3)

(OD FINISH RIGHT - 35 DEG. INSERT - VNMG-431)

G00 T303

G97 S3600 M03

G42 G00 G54 X0. Z0.1 M8

G50 S3600

G96 S500

G99

G01 Z0. F0.005

X1.12

X1.18 Z-0.03

Z-0.22

X1.45

Z-0.34

G40 X1.5914 Z-0.2693

M9 (No retract move)

G00 G28 X0.0 (BANG)

M01

 

(T11 OFFSET - 11)

(CENTER DRILL- .25 DIA.)

G00 T1111

G97 S1000 M03

G00 G54 X0. Z0.25 M8

G99

Z0.1

G01 Z-0.2 F0.004

G00 Z0.25

M9

G00 G28 X0.0

G28 Z0.0

M01

 

(T9 OFFSET - 9)

(9/32 DRILL)

G00 T909

G97 S1800 M03

G00 G54 X0. Z0.25 M8

G99

Z0.1

G01 Z-0.4545 F0.005

G00 Z0.25

M9

G00 G28 X0.0

G28 Z0.0

M01

 

(T6 OFFSET - 6)

(OD GROOVE LEFT - NARROW INSERT - GC-4125)

G00 T606

G97 S447 M03

G42 G00 G54 X1.71 Z-0.455 M8

G50 S3600

G96 S200

G99

M36

G01 X1.51 F0.0025

X-0.02

G40 X0.18

G00 X1.65

M9

M37

M33

G00 G28 X0.0

G28 Z0.0

M30

%

 

 

This just started today. I have not changed a thing.

 

Also, When posting, in the post dialog box, now it wants to save teh NCI and ask me about that. It also wants to ask about the NC file. I have always had those turned off in the machine def.

I run enough jobs through here that I don't have time to read every line of code. I used to have confidance in my code. Not any more.

 

This is going to QC as well

 

Rant off....

[dan m]

Just curious shouldn’t G28 be a U0. instead of X0. ?

[ATG]

I would imagine this is a boring bar. I've had this happen a couple times also. Now I’ve resorted to putting a retract point on every boring bar op that I run.

[BrianCNC]

That should be G28 U0. G28 X0 will go to machine zero on the X, but it will go to X0 on the part first.

[chris m]

No help on your actual problem, but I use ref points for approach and retract for every tool in every program I write; helps to keep me out of this type of thing

[mike_f]

I've hard coded a G0 Z.5 in my ptoolend$ section

in some of my lathe posts to avoid that.

 

like this

 

code:

---

pbld, n$, "G0 Z.50", e$           

if posttype$ = two, pl_retract

else, pm_retract

if n1_gcode <> 1003,

---

the only bad thing is if your tool is inside a groove or recess...you would need to watch that, that could be bad.

I try not to hard code moves like that because then MC doesn't know where your tool is.

[crazy^millman]

Mike that is really bad advice and I would suggest no one do this. I set Z at the back of a part middle of a part or front of a part and as Chris said Ref points are your best friend when doing any id work. Also I use them when doing any tailstock work. Reminds me of the days when I use to program and Quickturn and put my move in the TPC verse relying on the define the tailstock on a Mazak to avoid crashes. I tell it where I want it to go I know it goes there. Anytime you turn control over to the machine asking for trouble why I hate canned roughing cycles.

[chris m]

I with Ron on the hardcoding; I have stuff programmed from the chuck jaws and from the face so a hardcoded move like that would be a kablammo situation. My only word of caution about ref points is that there was a canned cycle posting bug in V9 that didn't output retract ref points when coming out of a canned cycle. The bug is fixed in my posts but I'd suggest carefully looking at your output after canned cycles the first couple of times through.

 

C

[dan m]

I used to use ref points all the time but since I started using stock boundries I have not had any problems.

[mike_f]

official retraction:. ...Ron you are 100 percent correct.....this works for me, in MY situation. on ONE of my machines, I have a seperate post for when I use the tailstock to retract to z.05

like I said, I don't like to hardcode moves in a post, it's a bad practice and I wouldn't recommend it. I'm glad you brought it up.... again, this works for me and I didn't intend to recommend anyone else do this.

in this shop Z zero is the face of the part 100% of the time, no exceptions, ever. I put this in because I forgot to set a ref. point once and tried to retract a 2.00 dia. boring bar to my X ref. point from 4.00" inside a bore it wasn't pretty and I didn't ever want it to happen again.

Thank you for pointing out what the some of the consequences could be...

[calnet42]

I ALWAYS run EVERY prog through InPlot, saved my butt more times than I can remember.

 

Mastercam is not a WYSIWYG program.

 

Inplot also can check syntax like coolant, feed without spindle on, "O" in prog etc....

 

The prog. only costs $150.00, real cheap insurance!

 

i-logic web page

[Thee Dragracer1951]

Thank you Gentlemen for looking at this.

This is a Haas SL10 and I've never used U's and W's for this machine. I have only used G28 Z0.0 and G28 X 0.0 to put the turret home. My issue that has just cropped up today is that it's not posting any retract moves to a positive Z position after the G40 move. So, It I turn off comp at a negative Z position, it'll crash because there is no G00 Z.25 or so in there...

This is a new thing that just started happening.

My Daewoo uses U's and W's. It's a Fanuc control but I've never used them with my Haas.

Not sayin that ain't the problem...but it hasn't been in the past.

[YoDoug®]

+1 to the ref points. Been burned by this myself a time or two.

 

Also don't trust verify in lathe, it doesn't show retract moves. I only trust the backplot because I can see the rapid moves.

[crazy^millman]

Glad you took it as it was. I have seen I have done it with tools myself. I just see someone half reading this thread seeing that putting it in their post and then crashing a machine and going to their boss well Mike F on the forum did it that way.