Quick question from a lathe nOOb.

I am going to make 5 parts on my TL-1. It's going to have a few turned outside diameters in progressive steps and three bore diameters.

Since I'm going to have the boring tool touched off and in the tool holder anyway, I'd like to bore the center, then reverse the spindle and do all of the OD operations with the same tool (on the backside, spindle running backward).

How do I address those coordinates? Negative radius? If I use G71, 72, or 73, do the X-steps also become negative to invert their direction? Or is this a case where I want to do a mirror operation? And if so, do all of the coordinates remain positive then?

Thanks in advance

Are you sure you have enough X travel to do that with a standard bar?


Here's a tool designed for easily doing what you describe. It works well if your workpiece is a good fit.


http://mrainey.freeservers.com/Miscellaneous/BoringBar.jpg

Yup, plenty of travel.

Donkey, piece of cake.
Pick up your tool just as you normally do, and program the OD with the positive X dims, and when moving to the ID just reverse the spindle and program as -X.
Here is a quick example for a 2" od roughed to 1.5 and a 1" ID rouged to 1.25

G00 G97 T101 S600 M03
G00 X2. Z.05
G96 S300 M08
G71 D.1 P10 Q50 U.01 W.003 F.01
N10 G00 X1.
G01 Z-1.
N50 X2.
M05
G00 X-1. Z.05 (MOVE TO BORE)
G96 S300 M04 (REVERSE SPINDLE)
G71 D.05 P100 Q150 U.01 W.005 F.008
N100 G00 X-1.25
G01 Z-1.
N150 G01 X1.
M09
M05
G28

Note that in this case U was positive in both cases, as it is defining the direction of the allowance.

Now if you were using Mrainey's tool, you can make it sing really sweet as it can not only rough OD and ID, but also finish OD and ID. In other words that one tool would replace 4 separate ones for 4 separate operations.

Thank you kind sir. :)

Yes, new tools are wonderful. Right now, I am trying to get by with what I have. There are some really innovative tools out there for this kind of stuff.

I'll give it a try tonight or tomorrow and post the results.

...

G00 G97 T101 S600 M03
G00 X2. Z.05
G96 S300 M08
G71 D.1 P10 Q50 U.01 W.003 F.01
N10 G00 X1.
G01 Z-1.
N50 X2.
M05
G00 X-1. Z.05 (MOVE TO BORE)
G96 S300 M04 (REVERSE SPINDLE)
G71 D.05 P100 Q150 U.01 W.005 F.008
N100 G00 X-1.25
G01 Z-1.
N150 G01 X1.
M09
M05
G28


Hope you have not copy/paste that code at tested it at 100% rapid feed.

Haven't even got that far. Waiting on a bar of material and for somebody to turn on the sales order. It came to me as an emergency, rush-rush job and now I've heard nothing for 4 days. The wheels turn mighty slow in aerospace.

Oh, and there is lesson #2: Always graph your program first, then run with coolant off with a 2" added to your Z workoffset.

Seems lately my fingers gettin' thicker and thicker....

Sorry 'bout that!

Thanks for the additional tips. Yes, I've already figured out that running the part with 5" of extra Z is a nice way to prove it out and still leave enough time to slap the E-stop button if something goes amiss.

(and you know I'm still gonna' crash it one of these days :D)

And also, when you are prepared to do a "cut-air verification run", to loose less time you could use the dry run button. But usually, the graph mode is enough to know if your prog is right or wrong.

And yes you will crash it someday for sure like probably everybody.

There is only one problem with Dry run, Haas or otherwise.
You will inevitably type .1 instead of .001 sooner or later for a feedrate, That soes not show up on dry-run.
Done that a couple of time at the beginning, but after the second or third oopsie I've decided the extra 3-4 minutes is well worth it.
Not to mention the ability to see the small nuisances with tool retraction during no-room bores, up-at-the-wall faces, grooves etc.

This is why I wish Haas had a little better graphing, or better yet, graphing on the PC.

Wouldn't you have to turn off the h&T agreement so you can compensate for direction and wear since you would have two different touch offs and geometries for the same tool #?

Nope.
First, it is the same touch-off. Once is used on the OD with positive X, the other is on the ID and is a negative X of the very same pickup.

What you're thinking is if the double inserted tool picked up separately for each insert. Even in that case the lathes don't care about the offset calls, and that option is only available for the mills.

Yeah, I had the double sided tool stuck in my head.

Just to add to this (since it was brought up), the current TL series software does have H&T agreement as a setting. A two-sided tool (or multiple gang tools) can still be used though and that setting can be left on.

There is now a setting for 'changer type'. The choices are (I'm doing this from memory so the words may not be exact): Tool Post, Turret, Gang.

If the machine is setup with multiple gang tools (such as the two-sided Dorian mentioned earlier), the control can be set to 'gang' and it will simply switch offsets when the next tool call happens.