Delivering Customized Solutions

Choose an Advent thread mill that best fits your application. Consider the number of parts or holes that are being produced. In the case of larger lot sizes, cycle time may be an issue along with tooling cost. This is where a single or multiple flute replaceable insert thread mill would be your best choice. The main advantage is the ability to change out inserts quickly and inexpensively while utilizing the benefits of wearability inherent in carbide. In the case of smaller holes where replaceable indexable tooling is not available you should consider solid carbide or carbide tipped tooling.  Our multiple flute carbide thread mills are made of the finest quality sub-micron material and CNC ground to maintain tool quality and pitch diameter repeatability.  In short, we provide for an excellent platform from which to mill threads or other forms.  However, there are several considerations that must be taken into account to get in the ballpark with the right tool.

Consider

• The major and minor diameter of the thread to be milled
• The length of the thread form
• The pitch (number of threads per mm or inch)
• The material to be thread milled and its inherent properties
• The quality of your fixturing and machining center for rigidity
• The amount of tool extension.  The shorter the better

Thread milling requires the use of a machining center capable of helical interpolation. This means the machine must be capable of three-axis simultaneous movement. Two of the axes perform a circular movement around the center of a plane while the third axis moves perpendicular to the circle's plane the equivalent of one pitch in a 360 degree circle. For the most part this is achieved by using a G02 or G03 command.

Due to the cutting action of a Thread Mill the forces acting on the part differ greatly than those due to tapping. The more rigidly the part is fastened to the fixture the faster you can Thread Mill. The speeds and feeds are maximized when vibration of the part and fixture is minimized. The next factor of the utmost importance, is the tool, and tool holder. The speed and feed are reduced depending on the distance a tool is held from the spindle face. If you consider the rigidity of your fixture, and the distance of the tool from gauge line, you should not have a problem with any thread milling operation.

Feed Rate Calculation

Due to the circular motion of the cutter as it forms a thread the actual feed rate at the cutting edge will be different from that which is programmed at the center of the tool. Straight line milling is a straightforward calculation.  Feed (F) = Rotations Per Minute (RPM) X Number of Flutes X Chipload Per Tooth.  For an internal thread the feed rate at the edge actually increases as the cutter diameter increases. For an external thread the feed rate at the edge decreases as the cutter diameter increases. This can be shown as a direct relation between the size of the circle the cutter moves within.  There is a formula used to calculate this and basically we calculate what the actual feed rate is at the cutting edge in order to tell the machine at what feed rate we want the centerline of the spindle to move.  So, once we calculate what chipload and feed rate we want - based in a straight line - we mathematically determine the feedrate to program the machine - because it really doesn't know what you are doing.  The formula is as follows...  

Internal Thread:  

Feed Rate to Be Programmed = Actual Feed Rate X (Diameter of the Work - Diameter of the Cutter) / Diameter of the Work.

External Thread:

Feed Rate to Be Programmed = Actual Feed Rate X (Diameter of the Work + Diameter of the Cutter) / Diameter of the Work.