Threading
This section is intended to assist in calculating the correct parameters for cutting both straight threads and standard NPT pipe threads using the system. First, an overview of general thread cutting using the system will be outlined. There are three things the user must define in order to properly cut a thread using the system: what kind of thread to cut, how to cut the thread, and where to cut the thread.
Thread Dimensions - Defining the kind of thread to cut
Style: This pop-up menu is used to select the thread style, such as UNF, NPT, etc.
Nominal Xd: This is the nominal thread diameter.
TPI: This is the number of threads per inch, (per millimeter for metric parts). This value should only be in millimeters if the actual part file itself has been designated as a millimeter part. If a metric thread is being cut, and the part file itself is set to inches, then the thread pitch must be converted from millimeters to inches and input as threads per inch.
Taper (Slope): This is the decimal slope of the thread taper, measured radially. For straight threads, this value should be zero. For standard NPT pipe threads, this value should be 1/32 or 0.03125 (the slope of NPT threads is 1/16 of an inch per inch on diameter, which is 1/32 of an inch per inch radially). If you are creating a tapered thread with Run In, Canned Cycles should not be used. This is because most machines cannot handle this situation.
# of starts: This is the number of thread starts. For multiple start threads, enter the number of starts here. Otherwise, this value should be one.
Major Xd & Minor Xd: These values will default to the theoretical major and minor diameters based on a perfect sharp thread. The value as calculated is primarily for reference; this value can be changed as required for the particular thread class and fit desired. For OD threads, the minor diameter is critical as this will be the diameter that the tool will cut on the finish pass. On ID threads, the opposite is true. The major diameter is critical as this will be the diameter that the tool will cut on the finish pass of an ID thread.
Thrd Ht Xr (Thread Height Xr): This value is the actual thread height as a radius dimension. This value is calculated as the radial difference between the Major Xd and the Minor Xd and can be changed as required.
Cut Information - Defining how to cut the thread
Cuts (Z-, Z+): This is used to specify the direction of the thread cut; Z- will cut toward the spindle and Z+ will cut away from the spindle. The Z- choice is the default as most threads will be cut toward the spindle; only in rare cases is the Z+ option used.
OD, Front ID (Approach Type): This is used to specify whether the user is cutting an external or internal thread; the type of thread will affect the approach moves to the thread cutting cycle. It is also correct to think of this as the Thread Type.
In Feed - Balanced: This choice will feed the thread tool straight in for each pass resulting in both edges of the thread tool cutting equally.
In Feed - Thrd Angle (Thread Angle): This choice will cause the positioning move at the start of each pass to feed the thread tool in at the angle specified, resulting in the leading edge of the tool doing most or all of the cutting. It is common to set the in feed angle slightly steeper than the thread angle so that the trailing edge of the tool takes a `light' cut to ensure that the back side of the thread cleans up.
T I P
This option is often used to improve the chip flow on soft or gummy materials that tend to tear during the cutting cycle because of material load up on the tool
Alternate: This option is only available when the Thrd Angle is selected for the In feed. It will alternate the in feed, resulting in the tool first cutting with the leading edge, then alternating to the trailing edge, and then back to the leading edge, etc. This provides even tool wear, in turn providing maximum tool life.
Depth Of Cut
The values and options in this section of the Thread dialog are used to control the number of cuts as well as depths of cuts, minimum cut depth, and spring passes.
1st Xr: This value is the stock amount to remove on the first rough pass. This value also controls the entire roughing cycle as described below for Constant Cut and Constant Load.
One Finish Pass: This option specifies that the tool only take one cut at the finish thread depth. This would normally be used to re-cut a thread as part of a de-burring process.
Const Cut (Constant Cut): The Const Cut option will cause the roughing cycle to step in the amount specified in 1st Xr on each subsequent pass until the tool reaches the Last Cut amount. A larger 1st Xr will result in fewer passes, while a smaller 1stþXr will result in more passes.
Const Load (Constant Load): The Const Load option is the most commonly used type of thread roughing cycle. This cycle will take a constant volume of material on each pass, resulting in a smaller depth of cut on each subsequent pass until the tool reaches the Last Cut amount. The volume removed on each pass is calculated based on the depth of cut specified in the 1st Xr field. This can also be considered a constant amount of tool pressure.
Last Cut: When selected, this option will prevent the roughing cycle from taking any rough passes at less than the value specified. In addition, the rough cycle will always leave exactly this amount for the last pass.
Spring Pass: This value is used to specify whether to take one or more spring passes at the finish depth.
Thread Location - Defining where to cut the thread
Thread Start Z: This value is used to specify where the actual thread begins in Z. If a thread begins at the face of the part, this value should be Z0; note that this is not the Z start of the thread cycle.
Thread End Z: This value is used to specify where the thread ends in Z.
Z Run In: This is where the user specifies the acceleration distance, incrementally. For example, if the thread cycle is to start 3/10" before the actual thread start, simply enter 0.300 for the Z Run In.
X Run In: This value would be used to specify an X acceleration value if necessary. Note that this value should normally be zero.
Z Run Out: This value will extend the thread by the amount entered. If the threading tool needs to pull out from the thread on an angle, enter a value for the Z Run Out and the X Run Out. Typically, a zero would be entered.
X Run Out: When used with Z Run Out, will cause the tool to pull out of the thread on an angle. For example, to specify a thread pull out of 3/20" at 45 degrees enter 0.150 X Run Out and 0.150 Z Run Out. A pull out move at 45 degrees for a distance of 0.150 will be added to the thread cycle.
Cutting standard NPT Pipe Threads
The primary problem that most people encounter when trying to cut pipe threads is determining the correct Major or Minor diameter, which is necessary in order to program the tool path. Unfortunately, the Machinery's Handbook does not supply these numbers. It provides the pitch diameter, and the major or minor diameters must be calculated accordingly. This becomes tricky due to the fact that all of these diameters are at an angle; therefore, these values will change depending upon the horizontal Z value.
Step by step instructions will be provided for programming both a 2.5"-8 NPT external and a 2.5"-8 NPT internal thread to show the actual process required to determine the minor and major diameters.
First, a given horizontal value must be established to act as a gauge point. Since the Machinery Handbook supplies the pitch diameter at the start of the thread, the horizontal value most commonly used is Z0 (the face of the part). The system also assumes this value for the major and minor diameters, and will calculate the major and minor diameters at the start and end of the toolpath based on this assumption. The advantage of this is that only one value needs to be calculated; in the case of external pipe threads, only the minor diameter at the face of the part is needed, and with internal pipe threads only the major diameter at the face of the part is needed.
2.5" - 8 NPT EXTERNAL PIPE THREAD
1 Find the Pitch Diameter at Beginning of External Thread (E0) from Machinery Handbook: American Pipe Threads: Table 3 (Basic Dimensions, American National Standard Taper Pipe Threads). For a 2.5" - 8 NPT external thread this value is 2.71953
2 Find the nominal truncated Height of Pipe Thread (h) from Machinery Handbook: American Pipe Threads: Table 1 (Limits on Crest and Root of American National Standard Taper Pipe Threads). This value is given as a max/min dimension; add the minimum and maximum height and divide by two to obtain the nominal thread height. For a 2.5" - 8 NPT external thread this would be (.1000+.09275)/2 or 0.096375
3 Find the Minor diameter at the start of the thread. To calculate this value, simply subtract the nominal thread height from the Pitch diameter (E0). For a 2.5" - 8 NPT external thread this would be 2.71953 - 0.096375 or 2.623155
2.5" - 8 NPT INTERNAL PIPE THREAD
1 Find the Pitch Diameter at Beginning of External Thread (E1) from Machinery Handbook: American Pipe Threads: Table 3 (Basic Dimensions, American National Standard Taper Pipe Threads). For a 2.5" - 8 NPT internal thread this value is 2.76216
2 Find the nominal truncated Height of Pipe Thread. This value does not change for external and internal threads and is the same as the 2.5" - 8þNPT external thread above (0.096375)
3 Find the Major diameter at the start of the thread. To calculate this value, simply add the nominal thread height to the Pitch diameter (E1). For a 2.5" - 8 NPT internal thread this would be 2.76216 + 0.096375, or 2.858535
American National Standard Taper Pipe Thread (NPT) Chart
This is a simple chart containing the values for the Standard NPT Pipe Thread sizes. For an external thread, enter the Minor diameter as given on the chart, and for an internal thread, enter the Major diameter as given on the chart.