How do I edit my code so the threading tool takes a couple passes at final depth? In effect, I'd like to have a couple spring passes.
Also I'm pretty sure there is a way to have the same tool just skim the major dia. to reduce burrs at the crest of the thread, but I can't find the info in the manual.
Sample of OD threading code:

N129 (OD THREAD)
N130 T505
N131 G54
N132 G97 S500 M03
N133 G00 X0.644
N134 Z0.2476
N135 G04 P1.
N136 M09
N137 M24
N138 G76 X0.483 Z-0.54 K0.0505 I0. D0.005 F0.0492
N139 G00 X0.644 Z0.2476
N140 M09
N142 (RAPID)
N143 T505
N144 G54
N145 G00 X3. Z10.
N146 M00

Thanks, Greg B.
Also thanks to all the folks who have answered my other questions on the forum. It's been a big help.

G76 is one way to make threads, but have you tried a G92??

I've been looking over the G92 option. Seems like alot of extra code to write. But I can see how it gives you finer control over the threading passes.
The code in my previous post was generated using the Haas IPS threading feature.
I have literally just started learning this machine, and I've never run a CNC lathe before. Just getting this far has been a bit frustrating but like I said, folks here have been really helpful.
Greg B.

Take the time to learn G92, it gives you much more control and allows you to tweak the size just by changing the X coordinate in your final passes. And it is really not that much extra code; write the G92 line and the following line with just the X coordinate, select and copy the X line six to ten times and then just step down changing the X values.

So if I were to try with a G92 the code should look like this?
M14 X 1.25 thread, by the way.

N129 (OD THREAD)
N130 T505
N131 G54
N132 G97 S500 M03
N133 G00 X0.644
N134 Z0.2476
N135 G04 P1.
N136 M09
N137 M24
G00 X.644 Z0.2476
G92 X0.540 Z-0.54 F0.0492
X0.535
X0.525
X0.515
X0.508
X0.501
X0.495
X0.490
X0.487
X0.485
X0.484
X0.483
X0.483 (two passes at same dim.)
X0.545 (pass to skim thread crests, or is this not allowed?)
N140 M09
N142 (RAPID)
N143 T505
N144 G54
N145 G00 X3. Z10.
N146 M00

Thanks, Greg B.

Your 0.545 pass will not do anything because the tool is aligned with the root of the thread not the crest. If you want to skim the crest you need to move you Z starting point by half a pitch.

But I don't quite understand what you are trying to get by skimming with a threading tool, surely you need something with a flat end such as a narrow grooving tool?

Of course the best approach is to use a full profile thread insert.

Your 0.545 pass will not do anything because the tool is aligned with the root of the thread not the crest.

Geez, that was so obvious (after you said it, of course).
Sometimes I think if brains were dynamite I couldn't blow my own nose.
I'm using a single point insert, because that's all we have at the moment. And it does throw up a burr on the crests. My thought of using the threading tool was to avoid another tool change. We didn't get the turret option with our TL, but I kind of wish we had.
I suppose I could use the parting tool to skim the crests just before I cut off the part. Otherwise I'm ending up using some Scotchbrite after the fact.
Thanks, Greg B.

With a bit of experimenting you should be able to figure out the Z start position and the X coordinate to have the threading tool take a little chamfer cut along each side of the crest.

Alternatively just use the threading tool as a turning tool to take a finish pass along the thread at the OD and knock off the burrs. With this approach you can then go back and do a final clean up pass on the thread after taking off the burrs.

Tried the G92. Like it better than G76. More effective, and less cycle time. At least over the way the IPS figured the threading passes.
Had a few weird issues when I saved the IPS program back to the shop PC and tried to do some editing offline. Control wouldn't accept the program when I tried to send it back. I pretty sure I had something screwy in the file name, but I've yet to figure out what it is.Didn't like it coming from a USB drive either.
Ended up just redoing it with the IPS and making changes at the control, like taking out all the extra M00s ,adding M08s, & M09s where I needed them. And putting in the G92 stuff. Still need to edit out a bunch of unnecessary axii moves to make it run a little faster. BUT I did make some parts, finally.
Thanks so much for your help.
Greg B.

Check the % at the head and tail of the file when you load back to the machine.

Also check for long comments between parentheses, i.e. (COMMENT). I have found sometimes that the machine does not like a (COMMENT) that is long enough to line wrap. It loses the closing ) and alarms.

why dont u just turn it like a norml turniing after u have done the thread ?

G0 X0,6 Z0,2
X0,549 (= 13,95mm TIP OF M14 )
G1 Z-0,54 F0,008
G0 X1 Z1

:D

why dont u just turn it like a norml turniing after u have done the thread ?
:D


Hvordan har du deg,
(think I spelled it right)
That's pretty much what I ended up doing. Using my parting tool to just skim the threads at the major dia.
tusen takk
Greg B

Somewhat unrelated to the topic, but if I want to shift all my Z offsets 1/2" closer to the spindle face I would enter -.500 in the G54 Z offset column, correct? Right now X & Z are set to 0.0.
Also if I were to enter .002 in the X wear of tool 3, would it change the dia. of the part by .002 or .004?
Thanks, Greg B.

Yes, -0.5 in G54 moves everything toward the chuck 0.5.

Does wear apply to radius or diameter? I think it is probably diameter because the X offset values are diameter.

Thanks, Geof,
I was pretty sure about the G54 bit.
I'll try tweaking the X wear on tool 3 a little at a time and see how it turns out tomorrow.
Greg B.

.....I'll try tweaking the X wear on tool 3 a little at a time and see how it turns out tomorrow.
Greg B.

I have a thought here: Are you using tool compensation? Does the X wear do anything on a lathe when you are not using compensation?

I know on a mill that compensation has to be active for wear to work but on a lathe I so rarely use either compensation or wear I don't know if it is the same. And I am too lazy to pick up my manual and try to find it.:D

Looks like you don't need comp turned on to use the wear column. I changed the X wear by .010 and got a part that was .010 bigger on the dia. Entered a -.004 and got the part - .004.
Anyway, thanks to all the help I've gotten, I was able to accomplish this on Saturday morning.

http://img.photobucket.com/albums/v11/GregB/FeedthruBolts-1.jpg
http://img.photobucket.com/albums/v11/GregB/FeedthruBolts003.jpg

So, I'm pretty happy. But I know this is just the tip of the iceberg, so to speak.
These are relatively simple parts, I know. But for the first thing I've done on a CNC lathe.....well you know.
Greg B.