Thread Shape Parameters
Use the Thread Shape Parameters dialog box to tell Mastercam the shape of the thread that you want to cut. There are three main parts to this information:
- Geometry of the thread form. Mastercam gives you three ways to enter the dimensions. You can select the dimensions from a thread form table; compute them from a formula, or enter the values directly into the fields. Use the picture as a guide.
- Orientation of the thread. You can program threads on the ID, OD, or face/back. You can also enter a taper value, or cut threads from the other side of the X-axis by selecting the proper options. The guide pictures update as you make different selections.
- Thread allowance values. You can choose allowance values from a table, or enter the values directly.
Choose Draw Thread to preview the thread geometry in the graphics window. Choose Yes when prompted to save it with your part, or No to return to this tab without saving it.
Mastercam's stock preview functions only show the first and last threads to speed processing time during screen display. For purposes of collision detection, the thread is a flat surface across the tops of the threads. Select True Thread mode on the Data tab in the Simulator Options dialog box, and then use Mastercam Simulator in Verify mode to accurately simulate the threads.
Lead
Determines the distance a nut would travel if turned once on a bolt for a given thread. Enter a value in the field and select the proper units. Mastercam uses the lead value and the spindle speed to calculate the feed rate.
- threads/inch or threads/mm: Calculates the lead value in threads per inch or mm.
- inches/thread or mm/thread: Calculates the lead value in inches or mm per thread.
Included angle
Enter the value of the angle between sides of a thread measured in an axial plane.
Thread angle
Enter a value of the angle between one side of the thread and a line perpendicular to the thread axis.
Major diameter
Enter the thread's largest diameter without an allowance or tolerance applied, or click to select a location in the graphics window which identifies the diameter. It may be easier to have geometry on the screen so you will know which point to select.
Minor diameter
Enter the thread's smallest diameter without an allowance or tolerance applied, or click to select a location in the graphics window which identifies the diameter. It may be easier to have geometry on the screen so you will know which point to select.
Thread depth
The distance from the minor diameter to the major diameter. When a thread depth value is entered, the minor diameter is updated so the distance from the minor diameter to the major diameter is equal to the thread depth. When either the major or minor diameter changes, the thread depth is automatically updated.
End Position
Determines where on the Z-axis (OD, ID) or X-axis (Face/Back) the thread will end. Enter a value or click to select a point in the graphics window.
Start Position
Determines where on the Z-axis (OD, ID) or X-axis (Face/Back) the thread will start. Enter a value or click to select a point in the graphics window.
Thread orientation
Determines where to create the thread. Choose an option:
- OD: to thread the outer diameter of the part (for example, a bolt).
- ID: to thread the inner diameter of the part (for example, a nut).
- Face/Back: to create a face thread on the front or back of the part (for example, an interlocking part). The Face/Back option is unavailable for the ThreadC Add-In.
Cross centerline cut
Create the toolpath on the opposite side of the centerline from the selected tool. Mastercam automatically switches the directions of the spindle rotation, compensation, and entry/exit moves.
Negative X
Indicates that the thread will be cut on the negative side of the X axis.
Taper angle
Determines the angle you want on the thread. A positive value will increase the diameter from the start of the thread to the end of the thread. A negative value will decrease the diameter from the start of the thread to the end of thread. If you pick the start and end positions from the graphics window and there is an angle, this value is entered automatically.
Select from table
Displays a list of standard thread tables from which to choose. Mastercam automatically fills in the fields for the thread dimensions with values from the tables.
Compute from formula
Computes the major and minor diameters once you select the thread form and enter the thread's basic major and lead values.
Draw thread
Returns you to the graphics window and draws an outline of the thread. You have the option to permanently save the outline as geometry.
Large end of taper
Choose to define the major and minor diameters from the large end of the taper. Becomes enabled only if the taper angle is not equal to zero.
Small end of taper
Choose to define the major and minor diameters from the small end of the taper. Becomes enabled only if the taper angle is not equal to zero.
Select from table
Check to activate the Allowances fields. Click to open the Allowances Table, that displays a list of standard allowance tables from which to choose.
Major allowance
Determines the amount of clearance between mating parts when screwed together. For an ID thread (nut), the allowance is added to the major diameter. For an OD thread (bolt), the allowance is subtracted from the major diameter. This option is unavailable if you choose face/back orientation.
Minor allowance
Determines the amount of clearance between mating parts when screwed together. For an ID thread (nut), the allowance is added to the minor diameter. For an OD thread (bolt), the allowance is subtracted from the minor diameter. This option is unavailable if you choose face/back orientation.
Allowance tolerance
Determines the total amount that a dimension can vary, or the difference between the limits, such as the smallest shaft and the largest hole. For an ID thread (nut), the tolerance is added to the major diameter and minor diameter. For an OD thread (bolt), the tolerance is subtracted from the major diameter and minor diameter. This option is unavailable if you choose face/back orientation.





