Lathe retract amount bore bar (Crash)

[Darin]

Hello,

 

 

I noticed when I post my rough and finish bore bar code it doesn't read the retract amount on the tool data parameter page. Below is the code posted out.. The attached screen shot show my settings.. I didn't run this way so it didn't actually crash but it would have at the end when it went home.. The bore was still in the part as you can see.. What am I missing in the settings? Do I need a lead out? I don't use lead in and out much on lathe... Where does the post read the rapid z retract amount from? I am using mplmaster post and control file and using advaced 4-2 machine file...

 

 

Thanks

 

 

G54

N6 T0606

G18 G99

M901

M202

M202

G97 S1500 M03

M8

G0 X.9175 Z.17

G50 S1500

G96 S600

G1 Z.07 F.005

Z-2.6358

G2 X.855 Z-2.7031 R.0881

G1 Z-4.3906

X.8267 Z-4.3765

G0 Z.17

X.98

G1 Z.07

Z-2.6188

G2 X.8975 Z-2.6457 R.0881

G1 X.8692 Z-2.6316

G0 Z.17

X1.0425

G1 Z.07

Z-2.615

X1.0313

G2 X.96 Z-2.6225 R.0881

G1 X.9317 Z-2.6084

G0 Z.17

X1.105

G1 Z.07

Z-2.615

X1.0313

G2 X1.0225 Z-2.6151 R.0881

G1 X.9942 Z-2.601

G0 Z.17

X1.1675

G1 Z.07

Z-2.6148

G3 X1.1563 Z-2.615 R.0994

G1 X1.085

X1.0567 Z-2.6009

G0 Z.17

X1.23

G1 Z.07

Z-2.6079

G3 X1.1563 Z-2.615 R.0994

G1 X1.1475

X1.1192 Z-2.6009

G0 Z.17

X1.2925

G1 Z.07

Z-2.588

G3 X1.21 Z-2.6113 R.0994

G1 X1.1817 Z-2.5972

G0 Z.17

X1.355

G1 Z.07

Z-2.5156

G3 X1.2725 Z-2.5962 R.0994

G1 X1.2442 Z-2.5821

(.625 DIA BORE BAR VCMT 21-MF FINISH BORE I.D)

G0 Z.025 <--------------------------Where is it getting z.025 the rapid retract is set to .5---------------------->

X1.4663

G1 Z0. F.01

G2 X1.375 Z-.0456 R.0456

G1 Z-2.5156

G3 X1.1563 Z-2.625 R.1094

G1 X1.0313

G2 X.875 Z-2.7031 R.0781

G1 Z-4.375

X.8396 Z-4.3573

G0 Z-1.22 <-----------------------Crash..------------------Shouldn't this be my retract amount on the parameter tool data page .5?----------->

M9

G28 U0. V0. W0.

M05

M30

%

 

 

Thanks

[chris m]

Use Reference Point on the retract for any ID work, ALL of the time, whether you think you need it or not

 

Why do you have stock recognition disabled? Other than faster regens, nothing good ever came out of that.

 

C

[GoetzInd]

Use Reference Point on the retract for any ID work, ALL of the time, whether you think you need it or not

 

Big +1.

 

Mastercam seems to have a mind of its own sometime.

 

Mike

[Hardmill]

Use Reference Point on the retract for any ID work, ALL of the time, whether you think you need it or not

 

Why do you have stock recognition disabled? Other than faster regens, nothing good ever came out of that.

 

C

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

PEACE

[Colin Gilchrist]

For Lathe to "automatically" retract the tool, you need to define stock in your Job Setup, and it needs to be enabled in the Operation. You can also set "Tool Clearance" values for Rapid and Feed moves on the Stock Settings page. For tight ID work, I'd change these to .005/.005 to avoid having the retract move crash your boring bar.

 

As others have mentioned, setting Reference Points for any toolpath operation removes any uncertainty of where the tool is as before it does a toolchange. Reference Points allow you to set a "Starting point" and "Ending point" for each toolpath.

[Darin]

Great guys thanks... I will do all of that..

[Rocketmachinist]

Colin

 

I have this problem right now on X7. I have my stock defined and everything. It showed the bar boring the hole and retracting out and clearing fine. Then I went back in and shortened my lead out from .100 to .010. Next thing I know the bar doesn't retract at all and tries to home from z-4.8 inside the part. (Big crash) probably something you should look into.

[Guest]

If your lead in/out is shorter than your radius on your tool, you're going to have problems

[Rocketmachinist]

^ In what ways?

[Guest]

^ In what ways?

 

If you're rad is .015 make your move .02 and watch, then make it .014

[Rocketmachinist]

Are you talking about on the shorten/extend portion of lead in/lead out? Because I do know about it leaving the radius on the back side of your part that is suppose to be a portion of the selected contour.

 

I was talking about when I change the retract distance.

[Guest]

Yup retract distance

[Colin Gilchrist]

Regardless of the Lead In/Out, you should be using an Approach and a Retract Reference Point for ID work. Do you have both set to Z values that clear the part?

[Rocketmachinist]

Yea, that is how I solve the problem but it was just strange how I was able to write a bore program to cut without crashing, then go back and change one minor thing and it suddenly wants to crash. I had spoke to someone at IMTS a few years ago and they were saying that there were discussions about making a boring specific toolpath. Anything coming down the pipe as far as that goes.

[Colin Gilchrist]

I believe Lathe is getting some serious development. I can't really say what is happening, but you can learn a lot more about what is coming by joining the Beta program. If you had a file that worked, you change a parameter and it doesn't, then please send that into QC (at) Mastercam (dot) com and provide them with the before file, and steps to reproduce the issue, so it can be addressed.

 

As someone mentioned previously, the stock definition (and Lathe Stock recognition) is what was driving the retract behavior.

 

I highly, highly recommend that you use an approach and retract point on every single ID path you create, just for safety. If you use the Reference Points, you can avoid crashing when doing ID work. It's as simple as that. You can even set the Operation Defaults to have them on.

[JAMMAN]

I'm going to look at the approach and retract point things didn't know they existed. I have a 10" retract hardcoded in the post for my big lathes and a 3" for the small one. Never have crashed a boring bar on the way out.