Blunt Start theards

[DryRun]

I have to make 112 PCs out of bronze with a 1.5X11 blunt start thread any ideas about how to program it would be helpful i will be using a fanuc controlled lathe to do the job?

[Geof]

Do a search using "Higbee" it has been discussed in a few posts.

[One of Many]

Also known as a higbee cut. The thread is cut as usual, then the starting partial thread is removed by CNC milling(or lathe live tooling) down to the first full thread profile, be that internal major diameter or external minor diameter threads of any configuration. This leaves a slight radius(from the cutter OD) or taper at the first full profile thread end.

Look at fittings and such that are coupled often by hand. This reduces the risk of cross threading or damaged thread starts of less than a full thread.

DC

[DryRun]

Thinks for the info i checked out the higbee thread will try when i get the stock in next week

[Sump Cleaner]

Dry Run,

You can also cut a 'Higbee' thread on a lathe without live tooling. Cut the thread as you normally do and then recut it with a 'cut grip' or some sort of square tool untill the first thread is cut off and is blunt. make sure the rapid is set at 100% so the 'ramp' is steep. You can adjust the z start to line up the edge of the square tool with the root of the thread. Here is an example of one that we do in a puma lathe.

Hope this helps.

JK

Here is a snapshot of what you should end up with...



%
G20G40G80G97G99
T0202(SER 0750 K16)
(INSERT 16ER 11.5 NPT)
G0X-1.95M3S800
Z.3M8
G76P010060Q0150R0040
G76X-1.75Z-0.595P0695Q0100F.0869
G0Z0.5
G28W0
M1
G20G40G80G97G99
T0303(GHDR 19-3)
(INSERT GIP 3.00E-0.20)
G0X-1.95M3S60
Z.15M8
G76P010060Q0150R0050
G76X-1.75Z-0.138P0695Q0600F.0869
G0X-1.790Z-0.060S2000
G1X-1.695Z-0.013F0.005
X-1.400
G0Z.2M9
G28W0M5
M30
%

[camminc]

Anyone out there know the difference in programming, say standard gcode, between a full and partial profile insert? Possibly tell me the difference in the program? Thanks, Randy

[ProProcess]

The only difference will be in the turning. You will leave some material for the "Full Profile" insert to "Top-Off" as it cuts.

[camminc]

Hi ProProcess: Happy to met you

Thanks for the input. I am wondering? If you might be a programmer and know this kind of stuff. Is there an input in the software that will ask if it is a "Full Profile or Partial Profile insert"? To compensate the different radius on the end of the inserts to determine "Passes and depth"? In some instances the depth of cut will be varied enough to allow more passes due to the radius on the insert? Is this correct?

[ProProcess]

You're welcome for the input.
I am a programmer but old school MG code and Macro.
I would think that CAM would ask about the insert type or that it would be defined in a tool library or some such.
Otherwise the output could be errant as you've suggested.
Good luck.