Results 1 to 13 of 13
Thread: Roll Tap Tap Drill Size
03-19-2008, 12:31 PM #1
Roll Tap Tap Drill Size
I'm going to use a roll tap or thread forming tap on some spacers. The material is 1 1/4" round 6061 Aluminum. I'm expected to use a #10-32 go-nogo gage to check the threads. Some time ago, on this board, a few people suggested a roll tap to get the thread fit I need. i know you have to move up in tap drill size, but am at a loss for the tap drill size for a #10-32 thread. Can anyone give me some guidance on this one? Is there a table in the machinist handbook for example?
03-19-2008, 12:40 PM #2
Look in the Machinist Handbook under Cold formed threads.
03-19-2008, 01:40 PM #3
cold form tapping
Here's an online calculator to plug your numbers into.
A #10 is .190" dia. so that figures to be .174" for the tap drill dia. if you use the figures for a standard 75% thread. A #17 drill would be the closest size.
03-19-2008, 01:46 PM #4
Hole size is critical to get 75% thread, check before tapping. You might need to go up or down in hole size to get the right fit for the gauge. If you use the tailstock make sure it aligned with the pc.
03-19-2008, 09:45 PM #5
03-20-2008, 02:46 PM #6
Careful there. The Karl is using a thread forming tap. It displaces metal from the hole walls to form the threads. A standard nominal dia minus thread pitch tap drill leaves too much stock. The metal will flow into the tap thread space, jamming the tap, and possibly breaking it.
The starter hole for a thread forming tap has to be larger than for a thread cutting tap. The displaced metal fills the tap's thread space to about 75% or so. I suggest you try a few tapped holes in scrap starting with a tap drill = nominal dia minus 40% of the pitch. Most makers offer charts.
03-20-2008, 03:06 PM #7
My Dormer Drills wall chart gives the following formula for calculating the tapping drill size for roll forming taps:
D(inches) - 0.0068 x H / Threads per Inch
Where H is the percentage of thread depth required (usually 65%)
03-20-2008, 04:52 PM #8
Roll taps (thread forming)
Make the pitch diameter good because they don't cut. It's the minor diameter you have to watch. Way lube works pretty well with them.
03-20-2008, 11:04 PM #9
Good Evening, Good People --
This evening's sermon is given from high atop one of my very favorite soapboxes -- that understanding the fundamental geometry of the two most common threadforms, the Unified and ISO Metric threadforms, enables we of the proletariat to calculate thread-chart values for ourselves, in the absence sufficient reference material, without resort to memorized "magic numbers":
As Forrest Addy describes, the rule of thumb to calculate the diameter of a hole to be threaded by material-removing methods (a cutting tap, single-pointing, or milling) for single-start US Standard, Unified, and ISO Metric threadforms is "Nominal Major Diameter minus Pitch". Either metric or imperial units may be used, but the same unit must be used for both Major Diameter and Pitch.
A corresponding rule of thumb to calculate the diameter of a hole to be single-start threaded with a Unified or ISO Metric threadform forming tap is "Nominal Major Diameter minus the Single Depth of Thread", which is itself calculated from the basic threadform as "5/8 Pitch times Cosine 30 degrees". (Remember that the basic forms of the Unified and ISO Metric screwthreads are IDENTICAL . . . they both have a 60 degree flank angle, a 1/8 Pitch flat at the Major Diameter, and a 1/4 Pitch flat at the Minor Diameter.)
I'll use a #10-32 Unified screwthread for a worked example:
Nominal Major Diameter = 0.190 inch;
5/8 = 0.625;
Pitch = 1/32 inch = 0.03125 inch;
Cosine 30 degrees = 0.866025.
Hole Diameter = Nominal Major Diameter - 5/8 Pitch x Cosine 30 degrees
Hole Diameter = 0.190 inch - 0.625 x 0.03125 inch x 0.866025
Hole Diameter = 0.190 inch - 0.016915 inch
Hole Diameter = 0.173 inch after rounding to 3 decimal places.
03-21-2008, 01:43 AM #10
I didn't read the whole thread but I've usually heard TDS for roll taps is right around pitch diameter. Usually best to try one in a piece of scrap first and see what the final ID is, it usually has a fairly open tolerance anyway.
03-21-2008, 02:13 AM #11
03-21-2008, 02:52 AM #12
Here is a simple chart that has percentage of threads for cut and formed threads. This data is from several sources and is one of those long hair academic exercises; There is source material that was traced. This chart is updated and expanded about once a year to include the latest bastard and obsolete information.
Hey; its free.................http://www.molineparts.com/images/36x96.pdf
Break out the magnifying glass if you print it out normally. This chart is 24" by 70" in normal size. When it prints you can hear the ink being sucked down as the plotter grinds on.
03-21-2008, 01:56 PM #13
For thread forming #10-32 holes in 6061 T-6 aluminum stock, I usually use a 0.177" drill (IIRC that's a #16). If your fit class is tight, I'd start in scrap with John Garner's info in post #9 and start out with a 0.173" (#17) and then check it against your gage.
Gotta love them roll forming taps. It's been years since I broke a tiny tap.