PIPETHRD

Tapered Thread Milling CNC Code Generator
Version 3.25
www.cncsnw.com

Installation

Insert the PIPETHRD diskette in the floppy drive of your control
Press F7 for the Utility screen
Press F2 for Update
When the "Installation complete" message appears, press ESC to return to the Utility screen, then press ESC again to return to the main control screen.

Running PIPETHRD

From the control's main screen, press F5 for CAM, then press whichever function key is shown for PIPETHRD. This will often be F4, but depends on what other software you have installed on your control.

Special Note for Windows CNC10 Users:

On Windows-based CNC10 controls the F5/CAM menu cannot be extended to include PIPETHRD. Instead, use a desktop shortcut to launch the program. The shortcut should run C:\CNC10\PIPETHRD.EXE, and should specify C:\CNC10\NCFILES as the working directory.

From the control software you can press F10/Shutdown, then F9/Exit to exit CNC10 and show the desktop. Double-click the PipeThrd shortcut to run. When you are done, double-click your CNC10 Mill shortcut to restart the control software.

PIPETHRD will prompt you for the thread milling parameters:

The XY coordinates of the center of the bore or boss.
The Z coordinate of the material surface.
The depth (down from the surface).
The clearance height (above the surface), for positioning before and after milling the threads.
The rapid height (above the surface); the cutter will move down to this height in a rapid move, then slow to the cutting feedrate for the remaining distance to the surface.
The diameter at the surface (minor diameter for outside threads, major diameter for inside threads).
The thread taper angle (half angle, in degrees; use 1.7899° for 3/4" per foot NPT threads)
The thread lead (vertical distance the thread advances in one turn).
The direction (right-hand or left-hand).
Whether to cut internal threads (in a hole) or external threads (around a boss).
Whether to start the cut at the top of the thread or at the bottom.
The cutting feedrate and tool number.
The number of cutting passes, and the depth (horizontal cut) to take in each pass.
The segment length. PIPETHRD will generate the spiraling path as a large number of straight-line segments. Values between 0.005" and 0.020" work well. Choose smaller numbers for better accuracy (but correspondingly larger CNC programs).
Whether to generate G codes with Absolute positioning or Incremental movement. Incremental is useful for producing thread milling subprograms which can be called at different locations. You should position the tool at the clearance height, over the thread center, before calling the subprogram. Program a G90 after the subprogram call if you need to restore absolute positioning.
The lead-in (and lead-out) distance for external threads. This must be greater than the cutter radius plus the thread height to avoid a crash.
The file name for the CNC program.

These parameters will default to whatever you entered last time you used PIPETHRD. If you do not need to change a value, just press ENTER to keep the default.

When you have entered all the parameters, press F10. PIPETHRD will write the CNC file, then return to the main control screen.

On DOS-based controls, the new thread milling CNC program is loaded automatically. On Linux-based controls and CNC10 Windows-based controls, The new thread milling CNC program is not loaded automatically. Press F2 for Load, use the arrow keys to highlight the new program's name, and press F10 to accept it.

The resulting CNC program will use cutter radius compensation (G41 or G42). You can, therefore, adjust the fit by changing the tool's diameter offset value in the Offset Library.

If you have problems with cutter compensation, try subtracting the cutter diameter from the thread diameter and using the diameter offset only for wear compensation (i.e. start with 0.0 in the offset, and add or subtract small amounts as needed to fine-tune the cut dimensions).

The header and footer codes (G codes inserted at the beginning and end of the program, respectively) can be customized.

On DOS-based controls, load and edit PIPETHRD.HDR and PIPETHRD.FTR, located in the C:\CNC7 directory.

On Linux-based controls and Windows-based controls, load and edit pipethrd.hdr and pipethrd.ftr, located in the c:\cnc10 directory.

In the header and footer codes, you may include the symbol %T any place you want to insert the Tool Number specified on the PipeThrd screen. All other codes are inserted literally, just as you type them.

Default header codes are:

  M6 T%T
  M3 S800

Default footer codes are:

  M9
  M5
  M25

Surface diameters for NPT threads

Size	Pitch	Int. Sfc.D	Ext. Sfc.D
1/8	.03704	0.3896	0.3475
1/4	.05556	0.5157	0.4533
3/8	.05556	0.6511	0.5880
1/2	.07143	0.8094	0.7275
3/4	.07143	1.0198	0.9367
1	.08696	1.2763	1.1760
1-1/4	.08696	1.6210	1.5195
1-1/2	.08696	1.8600	1.7584
2	.08696	2.3339	2.2314

These are approximate starting values. The surface diameter you need depends on thread mill tip geometry and thread fit requirements. As a rule, you will need to make test cuts in scrap material, starting small and working up, until you obtain the desired fit.

Legalese

I make no warranty, express or implied, with respect to their quality, performance, or fitness for a particular purpose. They are provided "as is", and you assume all risk associated with their use.

You should use all available means to verify that the job will run safely before you press the CYCLE START button. These include, but are not limited to, the F8/Graph and F6/Edit features of your control.

CNC Services Northwest Home