No retract in lathe (crash)

[nofalloff]

I saw Dragracers previous post about lath no retract.

No retract in lathe thread

 

I had the exact same thing happen to me today. ID boring, fanuc Oi control, MC post that I don’t use often but have used before (I don’t usually code for this machine). Post one program this morning fine, the second one, NO Retract at the end of the ID roughing. The machine just tried to rapid home from -1.75 inside the work piece. Snapped a .75 Sandvik carbide coolant through boring bar in half ($589) and scrapped the part. My program, so I was in the hot seat. Reposted the code in front of my supervisor and still no retract. Guess I will be putting ref points in from now on. A very expensive and embarrassing lesson. Why is it that there isn’t a retract or feed plane/point in each operation in lathe like there is in mill?

 

Maybe when they add in all those lathe enhancements in X3?

[Todd84]

I only use Lathe. I use it everyday. THIS HAPPENS ALL THE TIME!! It happens to me about 1-2 times a week. I am waiting for changes to happen. It is part of my routine to check and make sure there are retract moves on ID tools after I post. Sometimes it doesn't want to put them there. I was 10mm in a part yesterday and it wanted to send the drill home.

 

Sorry it just pisses me off when I hear this stuff

[chris m]

I always always always use ref points with ID and OD tools both, just to make sure that the tools are in a safe position before going home. Once you start doing it, it'll become second nature to you and will save you a lot of xxxx-ache

[gcode]

If you get in the habit of using the a Z reference point, his doesn't happen.

I use a z.250 in ALL operations approaching the part and leaving the part.

There is also a check box in Tool Settings

on the Machine Group Properties page named

"Write Home postion clearance moves"

it should be checked.

and finally

in backplot, make sure the "show rapids" button is pushed.

Before you post select all your OPS, go into backplot and hit the show all paths button..

If you've got a bad move you will be able to see it before you post.

 

and I always review the approach and retract moves in the posted code.. Cimco Edit 5.0 gcode backplot

is a lifesaver

[Steve Biehl - Cimquest Inc]

it sounds to me like you guys don't use the stock def in Lathe. If you set a stock def and talk the ops to use the stock def and update it then MC should not hit stock and willpull out of ID work before going home.

[Randy Morton @ Clem Industrial]

Funny, I have never had this issue and I use MC Lathe daily. I admit I do use ref. points (on Z only) for my approach and retract moves, but there is times that I happen to be speedily doing my work and forget to put one in...still nothing. Not OD/ID...nota. Never had it crash from that.

 

Now if you want to get me started on the G70 thing.........!!! That has caused a few good ones!

[chris m]

quote:

---

it sounds to me like you guys don't use the stock def in Lathe. If you set a stock def and talk the ops to use the stock def and update it then MC should not hit stock and will pull out of ID work before going home.

---

MC Lathe 9 regularly violates the clearance boundaries when roughing, and does rapid through the part on occasion, but I've never had a 'home run' move that would've wiped my part out which didn't generate a 'collision' message in MC EXCEPT for with canned cycles which had problems posting ref points.

[Thee Dragracer1951]

I'm going to have to go sit doen with my reseller and have them explain ref points I think. I have never been able to get them to work. (are we talking about home pos on the toolpath parameters page?)

I'm confused. I haven't had my coffee. I need a donut.

[gcode]

Directly under the comment box and just right of the tool display button. Its named Ref points.

If your Cplane is +D+Z it will show D and Z boxes

If you are in Top you'll get X and Z fields

 

You can make both lathe and mill

do all kinds of good stuff with

Ref Points once you learn the tricks

[Steve Biehl - Cimquest Inc]

quote:

---

MC Lathe 9 ...

---

Oh, I forgot, Chris the X hold out

[chris m]

That's right baby; I get paid to make parts, not find software bugs. Now that you guys pretty much have it figured out I'm going to have to convert...ugh

[Randy Morton @ Clem Industrial]

hahaha Convert to MCX2 on the 'so-called' verge of MCX3? lol That's funny

[Thee Dragracer1951]

Gonna be here any day now....

[Redfire427]

I'm sure there will be a huge improvement for lathe in version X3, er I mean, X4.

[nofalloff]

quote:

---

Directly under the comment box and just right of the tool display button. Its named Ref points.

---

Ref points? or coordinates?

[gcode]

Ref points

[gcode]

Steve brought up a good point.

If you don't define stock... its all just lines in

space and Mastercam will take the short route home

[Mick]

I never get rapid moves through the part, probably due in part to always using defined stock.

 

Without stock defined, you should ALWAYS use reference points. Steve is right, it sounds like stock isn't being used. If not, get familiar with reference points. They saved my bacon a few times.

 

On another note... I ALWAYS watch my retraction moves when proving out a programme.

[Thee Dragracer1951]

quote:

---

On another note... I ALWAYS watch my retraction moves when proving out a programme.

 

---

I do Now.....