Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations cowski on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
Machining for M18x1 Tap
- Thread starter garyhose
- Start date
eromlignod
Mechanical
- Jul 28, 2006
- 402
Since this is not a standard size, you have to calculate it based on the fit grade using formulas (which are in the Machinery's Handbook).
Not knowing your tolerance requirements, the minor diameter could be anywhere in the range of 17.06mm to 17.32mm.
Assuming that you just want to tap the damned hole and don't plan on boring it to exacting dimensions, I would recommend using a 17.25mm drill. If you don't have metric drills, try 43/64".
Don
Kansas City
Not knowing your tolerance requirements, the minor diameter could be anywhere in the range of 17.06mm to 17.32mm.
Assuming that you just want to tap the damned hole and don't plan on boring it to exacting dimensions, I would recommend using a 17.25mm drill. If you don't have metric drills, try 43/64".
Don
Kansas City
6H fit (medium)
min = 16.917 max = 17.153
4H fit (close)
min = 16.917 max = 17.067
75% thread = 17.025
Remember, your drilled hole will probably be larger than the drill by .05 - .100
Software For Metalworking
min = 16.917 max = 17.153
4H fit (close)
min = 16.917 max = 17.067
75% thread = 17.025
Remember, your drilled hole will probably be larger than the drill by .05 - .100
Software For Metalworking
eromlignod
Mechanical
- Jul 28, 2006
- 402
Remember that tap drill size and minor diameter, while related, are two entirely different things.
You can calculate and look up the fancy tolerances and dimensions all you want. But the actual thread you get is based on the tap itself. You can't really affect the fit grade by how big you drill the hole for tapping. The tap should be cutting both the crest and root of the threads, which determines their respective diameters.
The size of the drill hole is important in that it must be small enough not to truncate the crests, yet large enough to facilitate tapping and minimize chip production, torque and broken taps.
Don
Kansas City
You can calculate and look up the fancy tolerances and dimensions all you want. But the actual thread you get is based on the tap itself. You can't really affect the fit grade by how big you drill the hole for tapping. The tap should be cutting both the crest and root of the threads, which determines their respective diameters.
The size of the drill hole is important in that it must be small enough not to truncate the crests, yet large enough to facilitate tapping and minimize chip production, torque and broken taps.
Don
Kansas City
Sometimes you make threads for your own use, or have an understanding with your customer. That allows some liberties.
Other times you have to make them to a standard.
Minor diameters are a part of the standard, and an inspector can reject threads where the minor deviates from that standard.
Taps can be the right size and still make threads that don't gage correctly. Thus the popularity of thread milling - makes it easy to machine threads to the standard.
Software For Metalworking
Other times you have to make them to a standard.
Minor diameters are a part of the standard, and an inspector can reject threads where the minor deviates from that standard.
Taps can be the right size and still make threads that don't gage correctly. Thus the popularity of thread milling - makes it easy to machine threads to the standard.
Software For Metalworking
Garyhose - For gen. everyday taping inch or metric just use this:
Nom. Thread dia minus Pitch.
In your case: 18 minus 1 = 17 mm dia tap drill.
If you run into something like this: M8 x 0.75 = 7.25
just round it up or down to the next number =7.3 mm drill.
Forget about the second digit after a decimal point.
People not being able to think in metric will sometimes come up with up to three digits behind a decimal point. Usually that is a dead give away for a converted print. 1/1000 mm are for prec. grinding and lapping. Juergen
Nom. Thread dia minus Pitch.
In your case: 18 minus 1 = 17 mm dia tap drill.
If you run into something like this: M8 x 0.75 = 7.25
just round it up or down to the next number =7.3 mm drill.
Forget about the second digit after a decimal point.
People not being able to think in metric will sometimes come up with up to three digits behind a decimal point. Usually that is a dead give away for a converted print. 1/1000 mm are for prec. grinding and lapping. Juergen
- Status
Similar threads
- Locked
- Question
