[jimbo77]

Please help.!!

I am usung a cincinnati hawk turning centre with fanuc 21-t control.
i'm having a bit of trouble with a 1/2" NPT external thread. I have read previous problems that people have had with the 'x' dimension and the taper, but i still dont get it.

My threading cycle is as follows

T0300 (14 TPI)
X22.22 Z3.0 T0303
G76 P030060 Q100 R0.025
G76 X18.43 Z-19.05 R-0.672 P1450 Q100 F1.814
G00 X200.0 Z200.0 T0300
M01

i'm not sure how far from the face of the job i should start or how to work out the 'x' and 'r' values.

Any help would be really appreciated.

James

[g-codeguy]

What kind of material are you running? 03 means you are making 3 spring passes. Shouldn't need any. 00 means insert stays down one revolution at the end of the thread. This "rings' the thread. I use 01. This is the fastest you can make the insert pull out. Bigger the number the longer the pullout lead. 60 is the compound infeed. I use 60 only when trying to remove chatter. It has the least amount of tool pressure as the insert is cutting on the leading edge only. Try to avoid 60 when running work hardening materials. I would go with 29 or 55.

Start position should be at least Z7.62. I convert from metric, but not to metric, so hope I am doing the math correctly. In your example, I am getting R-.686, not really much difference.

Another forum member just posted a zipped spread sheet he uses for NPT threads. I laid out each size in MasterCam using data from The Machinery's Handbook. Not at work now so I can't check on your "X" value. If I need to thread deeper (or shallower), I then use trig to find the new X-value based on the one I've laid out in MasterCam. A sheet of paper in a desk drawer would work as well.

Taper (R-value) is simply tangent of 1 degree 47 seconds times the TOTAL Z-axis movement. Seems like you already have that down.

Dale

[jimbo77]

Thanks for all the info Dale

I am using 316 st/st.

The 'x' value seems to be the main problem here now. Working in imperial, am i right to believe that the o.d for 1/2" NPT is 0.840" and the final 'x' value is 0.840 minus x2 0.0571" (depth of thread) which would end up at X0.7258?

The only book I have on thread data is a pocket ref book. When I see other examples of NPT threads, their figures are slightly different to mine which could be my big problem from the start.


Many thanks

James

[g-codeguy]

You are correct that .840 is the O.D diameter.

No. X-value is not .84 minus 2*.0571. X-value is dependant on the ending Z-dimension (you are threading on a taper ). Your example should read X19.82 for a Z-19.05 value.

As you know 316 SS is a workhardening material. I would remove the spring passes if possible, and change the 60 to 55 or 29. I would also try changing R.025 to R.076 to keep a decent DOC on the last pass.

I have no idea how rigid your set-up is, size of tool being used, or how far the thread is from the chuck (collet). Start with those values, and experiment if necessary. Please let me know how it works out.

[chutch]

G76 P050160 Q0.005 R0.006
G76 X1.591 Z-0.410 P0.0695 Q 0.002 F0.0869

In the above example P060160 means :
5 = SPRING CUTS (05)
1 thread = CHAMFER AMOUNT(01)
60 degree = TOOL ANGLE (06)
Q0.005 = MINIMUM DEPTH OF CUT
0.006 = FINISHING ALLOWANCE
1.591 = ROOT DIAMETER
-0.410 = LENGTH OF THREAD
0 = THREAD RADIUS DIFFERENCE (*Straight Thread in this example)
0.0695 = THREAD HEIGHT (RADIUS)
0.002 = 1ST CUT DEPTH
0.0869 = THREAD LEAD

[cam1]

NPT threading......here's the attachement. I hope it serves you well.


regards

[cam1]

g-codeguy:
Mastercam already has all of the NPT threads in the library. I mentioned this to one guy recently, and he said "holy *&?*" I've been using it for all these years, and I never realized that all of the threads are in the library".

regards

[g-codeguy]

g-codeguy:
Mastercam already has all of the NPT threads in the library. I mentioned this to one guy recently, and he said "holy *&?*" I've been using it for all these years, and I never realized that all of the threads are in the library".

regards

Was just reading this post to see if anything had been added. We have been using Mastercam for many years. I knew that it contained standard straight threads. Never thought about it also containing NPT threads. I always manually program my threads. Actually I've always manually programmed, and use Mastercam whenever I would have to use trig otherwise.

That is changing as the company I work for wants all new programs done in Mastercam, and all repeat jobs done in Mastercam if they were originally programmed as a standard G-code program.

Thanks for the reminder. The other lathe programmer has always used Mastercam for all his programming. His thread cycles come out fine. However, I think he went through them, and changed some (or all) of the thread heights. Will have to remember to ask him about that.

Again thanks for reminding me that all the threads are already in Mastercam.

[cam1]

Cheers