Problem internal 1 1/2" -11 1/2 tpi npt thread cycle G&^

# Thread: internal 1 1/2" -11 1/2 tpi npt thread cycle G&^

1. ## internal 1 1/2" -11 1/2 tpi npt thread cycle G&^

wondering if any one could help with the bore size and final x position calculation for the above thread

the thread i am using is 1" long and i will start say .200" off the face of the job

i plan to use a 2 line g76 cycle

g76 P Q R
g76 X Z R P Q F

i am working on a fanuc based daewoo lathe

ive charts and date for most other section just struggling with these 2 values

a break down and explination will be greatly appreciated

new to this so go gental

cheers jc88

Similar Threads:

2. the NPT 1 1/2 - 11 1/2 thread dimensions are on many web site such as...
http://www.engineersedge.com/hardwar...pe-threads.htm
http://www.trentonpipe.com/ti_threadformdatachart.html
etc.

but it's not so easy to work it out because the major diameter is measured at a set gauge length not on the face or end of the thread. you have to work out taper and given major diameter subtract an amount from X based on the distance from gauge line at major diameter to face of part using trigonometry. this gives us the major diameter at the face. To calculate major thread X diameter at end of thread take the major diameter at face and subtract 2 * the taper amount over the thread cutting length but not from the start position, it needs to be calculated from the face.

taper is 3/4" per foot on diameter
taper per inch on radius = 0.03125
angle from centerline is 1.7899 degrees

for boring, X diameter at start of bore is major diameter at face minus 2 * thread depth.
so 1.8657 - (2*0.06957) = 1.72656
X diameter at end of thread is our G76 X value minus 2 * thread depth so X1.659. But you need to extend the length for boring a bit further for clearance so bore to about Z-1.2 and re-calculate the X using TAN(1.7899) * 1.2 = 0.0374 then subtract 2 * this number from the front X size.

Boring code....
G0 X1.7265 Z0.1
G1 Z0
X1.6515 Z-1.2

thread code....
G00 X1.4 Z0.2
G76 P020060 Q0.004 R0.001
G76 X1.6640 Z-1.0 R0.0374 P0.0695 Q0.01 F0.0869

1st line.....
P020060 = 2 finish passes, 00 = thread chamfer amount in pitch * 0.1 increments (i.e no thread chamfer), 60 degrees in-feed
Q = minimum depth of rough cuts
R = finish allowance

2nd line
X = diameter at end of thread
Z = end position in Z
R = taper amount across cutting length i.e. TAN(1.7899) * 1.2
P = depth of thread
Q = 1st cut depth
F = feed (1/TPI so 1/11.5)

These threads are a real pain in the ass because of the lack of machining dims on charts.
The basic dims for my calculations came from various places on the net so you may need to check/adjust them depending on the tolerances required for your thread. maybe it's completely wrong and you'll need to change everything ;-)

3. That's great. Cheers for the time
Jc88

#### Posting Permissions

• You may not post new threads
• You may not post replies
• You may not post attachments
• You may not edit your posts
•

### About CNCzone.com

We are the largest and most active discussion forum from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!