Home Position

[Rory]

In Lathe, where do I find the place to set up the "System Default" Home Position.

Its probably right in front of me but I cant seem to find it.

 

Rory

[d0gFartz]

from your Main Menu,Screen,Configure, then the NC Settings tab....its in the upper left

[Rory]

That was easy enough, Im supprised it didnt jump out and hit me.

 

Thanks

[McRae]

Rory,

 

Watch your approach and retract moves if you are using the home function. Practical experience will attest that tool holders will break in Rapid.

[GARRY P]

WHEN DOING A HOME MOVE BE SURE TO WATCH THE LENGTH OF ANY TOOLS LIKE BORING BARS STICKING OUT FROM THE TURRET. IF THE POST IS SET UP TO CANCEL OUT THE TOOL OFFSET THEN THERE IS A HIGH RISK OF CRASHING A BAR. WE DO A LOT OF LARGE TURNING AND I HAVE DISCOVERED THAT IF HOME POSITION IS X20. Z20. AND MY BAR IS HANGING OUT 25" THE OUTCOME IS QUITE FRIGHTENING

[Rory]

Garry,

 

Welcome to the forum!

 

Thanks for the input. It helps to get some advise.

 

Rory

[chris m]

Gentlemen

 

As Garry and Andrew have stated, home position returns can be scary if you don't have everything figured right. You may want to consider a "safe home" G-code macro or resident subprogram to safely bring your lathe to a comfortable tool change position regardless of tool size, part length, etc. You do, of course, need to have the tool out of the part before calling this. We have these in most of our lathes and they work well to avoid the thumps and bumps. It also allows your operators to call them in MDI which helps to avoid the overtravels and collisions that occur when guys are handwheeling or jogging the machine by hand.

[Rory]

Chris,

 

Would you be suggesting a sub similar to the following?

 

M98 P1

 

%

o0001 (SAFE START)

G0 G40 G97 G98

T0

X#501 Z#502

M99

%

 

The sub call could be inserted into the Post file as a literal string to replace the "Home Position" move.

 

Being as how this is a macro program the user can change the variables without touching the main program.

[chris m]

In a couple of our machines, as an example (Hardinges with Fanuc 18i-T) we use a G-code macro that looks like this:

 

quote:

---

%

:9010(SAFESTART/END PROGRAM)

N1M01

( SAFE START )

( WARNING )

(CLEAR ID TOOLS FROM BORE)

(BEFORE CONTINUING PROGRAM)

N5 G00 G40 G97 G80 G99 M11

N10 G50 S4000

N15 T0 G28 U0 M05

N20 G28 V0

N25 G110 T107

N30 G28 W0 M37

N35 G10 X0 Z0 P0

N40 T0

N45 M99

%

---

We use protected resident subs (.ssb) in some of the Okumas that are very similar.

 

C

[Rory]

Ok now I dont understand what is going on.

 

I have the home position set as X14 Z10.

We have a 10" chuck, yet when the machine pulled back to do a tool change it ripped the part out of the chuck.

When we look at the position (ABS & Machine)

It says its at X14 but it is really sitting at about 8". Why is the tool sitting at 8" and the machine reads 14"?

 

Rory

[McRae]

Your tool is programmed from the tip of the insert. The setup of the boring bar tool offset is what you are seeing.

 

Home position is very dangerous - watch the backplot before running the code on the machine. Another thing to do is to use ref points. This will add moves before and after the "Finish" contour tool path to prevent what just happened.

 

Another consideration is the tool lengths for setting your Z-Home, the longest bar is going to dictate how close to the chuck you can come with respect to turret index. For a turning tool, the home position may be 6" away from the face of the part but when you index your 7" long boring bar - it will interfere by 1" with the workpiece. As we said earlier, the home position is very difficult to setup.

 

[ 12-17-2002, 10:46 AM: Message edited by: Andrew McRae ]

[TheePres]

The Rapid feedrates on newer lathes are so quick these days. That I only use Machine Home on all Lathe programs.

[Rory]

I called Hardinge, and they told me the X coordinate comes from the center of the (VDI) tool holder pocket. Not from the tip of the tool as you would think.

 

So when I told it to go to X14 the center of the pocket was there but the turning tool was at around X8.

 

So I guess that means I got a "crash" course.

 

Rory

[McRae]

Now you got me. Are all your parts undersize by 6.0" in diameter when you bore?

 

This question may help, are you using a go home command or are you programming the X14.?

[Rory]

I'm programming the X14

 

"G0 X14 Z10"