(Or "Why do I always take 4 goes at a fit with G76") I recently had the occasion to think harder than normal about threads, and especially about their sizing and fits. Threads were one of the very first things to be standardised and made interchangeable, largely through the work of Josiah Whitworth. And it turns out that they are one of the more complicated things to standardise. The reason I was thinking about this was that I was trying to make a lathe faceplate for someone a few hundred miles away. I know that his spindle nose is 2 1/4" BSF. (ie, one of Whitworth's threads) but have nothing to use for a trial fit.
Whitworth threads have rounded thread crests and roots. ISO metric has flat crests and rounded roots, AN threads had flat roots, but that interfered with British rounded crests, so the Unified standard emerged which has flat crests and rounded roots. For a nut and screw to fit together there needs to be clearance between the thread flanks and also clearance between the roots and crests of both halves. This means that the roots of the internal thread need to be at a larger diameter than the crests of the screw, which also means a smaller radius or smaller flat. Similarly the minor diameter of the screw needs to be smaller that the through-hole of the nut. The flank clearance is assured by specifying different "pitch diameters" (or "effective diameters") for the internal and external threads. The pitch diameter is defined as the line through the thread where there is exactly as much air as metal. (ie, where the width of the thread is half the pitch.) Here is the data for the screw I was making, as an example: Size 2 1/4" BSF Internal Thread TPI: 6 Major Dia Min: 2.250 Effective Dia Min: 2.1570 Effective Dia Tol: 0.0137 Effective Dia Min: 2.1433 Minor Dia Max: 2.0769 Minor Dia Tol: 0.0403 Minor Dia Min: 2.0366 It is interesting that there is no limit to how large the major diameter of the internal thread can be. Presumably this means that it can be perfectly sharp. The "Effective Diameter" is the important measurement when inspecting threads, but isn't trivial because it is a measurement of an invisible feature. There are special thread measuring micrometers with a V anvil and point for measuring pitch diameter. And some maths is needed to interpret the reading. However each micrometer can only measure 3 or 4 specific pitches. A more accessible way to measure threads is with the "three wire method" where three short rods of known diameter are placed in the threads. Two on the top in adjacent threads and one at the bottom. The measurement over the wires is then taken with a conventional micrometer. Using this method the pitch diameter can be determined using some mathematics, here is an online calculator that I found: https://www.cgtk.co.uk/metalwork/calculators/screwmeasurement But, 1) I needed to make an internal thread and 2) I needed to make it before cutting it. 3) It isn't entirely clear what assumptions such calculators are making. So, here is another way. Firstly, it is possible, but even more fiddly, to measure an internal thread using ball bearings and an adjustable parallel. I was measuring quite a large thread so could use 3mm balls and a fairly big parallel. I drew the required thread in a CAD package, and used tangent circles to represent the balls. The pitch diameter in the drawing was set to the mid-point of the numbers from the standard. I set the thread angle in the drawing to 55 degrees. I probably shouldn't have; the perpendicular angle that defines the thread is a little larger than the angle along the thread. alpha = arctan(P / pi.D). the effective angle is roughly 55 - 1.4 degrees. And this turns out to make quite a difference: For 55 degrees and a min pitch diameter of 2.1433in the parallel would read 49.01mm For 53.6 degrees the parallel should read 48.976 But, the main point of this drawing was _not_ to work out how to measure the thread but how to make it. The crest radius on the male thread is 0.53mm on this size thread. The nut root needs to me smaller. I was using a Seco insert, and so had access to the data table, saying that it was a 0.5mm tip radius. I then drew the root of the internal thread at this radius, and measured the diameter that such an insert would bore at the nominal pitch diameter. Then at the machine, I used the threading insert to bore its own plain hole, and touched it off. I could then use G76 to thread out to the major diameter of the thread from the CAD drawing, being fairly confident that this would put the pitch diameter where needed. In the end it looks like I ended up on the large size, but inside the tolerance (helix angle?) which is probably where you want to be when fitting to a thread that you can't test to. -- atp "A motorcycle is a bicycle with a pandemonium attachment and is designed for the especial use of mechanical geniuses, daredevils and lunatics." — George Fitch, Atlanta Constitution Newspaper, 1912 _______________________________________________ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
