What's new
What's new

CNC Lathe: G76 threading for internal 1/4 NPT

DouglasJRizzo

Titanium
Joined
Jun 7, 2011
Location
Ramsey, NJ.
Ok, now the program runs fine, but the tool barely cuts anything. I double checked the tool offset and the thread dimensions and made an adjustment to the taper, but all it cuts at most is maybe a .005" scratch of a thread. I have to adjust the threader offset +.06" in X to get it to where its supposed to be. its doable since i have just over .08" of clearance to work with, but now its got me scratching my head again. I was aiming to taper the thread all the way to the drill diameter, but do I need to extend the z depth to do that? Or just bump up the thread endpoint by .06 in x?

Sorry if these questions seem stupid, but I've only ever worked with G92 threading cycles and we've always tapped NPT threads in the past, but we're trying to cut down on process steps and try and get as much done in one go as possible, but this is a bit of a learning curve for me


N5(THREADER)
G97S500M3T0505
G0X.335Z.2M8
Z.05
G76P020060Q010R.001
G76X.42Z-.55R.0375P410Q120F.0556
G0Z.2
Z.05
X6.Z6.M9
M1

I would get rid of that "Z.05" that's on a line by itself, for starts.
The X target is, .5025 according to my math - but I could be wrong.
The P word should be written out to four places - P0410 so should the Q - 0120
Get rid of the other Z.05 also.
 

SeymourDumore

Diamond
Joined
Aug 2, 2005
Location
CT
That is because of your X value!
That is what threw me in the first place for telling you to start at X.4.
You see, the .42 diameter of that thread is the MINOR, and that is NOT what you're shooting for!
The actual MAJOR dia ( which is your target ) you can calculate by X minor + 2X thread height - truncation at the crest ...
So, your .06 offset adjustment sounds about right.

Shoot for X.49 in your thread cycle.
 

angelw

Diamond
Joined
Sep 10, 2010
Location
Victoria Australia
N5(THREADER)
G97S500M3T0505
G0X.335Z.2M8
Z.05
G76P020060Q010R.001
G76X.42Z-.55R.0375P410Q120F.0556
G0Z.2
Z.05
X6.Z6.M9
M1
Hello crow71,
The taper specified is also wrong. The Taper is 1:16 measured in terms of diameter. The Taper amount specified in the G76 Cycle with the "R" address of the second G76 Block is the difference in Radius between the Start and End of the Taper. Accordingly, as the total Z length is 0.6" (Abs(Z-0.55) + Z0.05) then the Taper amount in Radius will be 0.01875".

Regards,

Bill
 

sinha

Stainless
Joined
Sep 25, 2010
Location
india
The easy-to-remember simple formula is R (magnitude) = L/32 where L is the total axial displacement.
 








 
Top