Tolerance of Thread Hole Depth

Look also at the cap screw that threads into this, and how much thickness of parts and washers it goes through first.

In addition, there may be a "default tolerances" statement on the drawing, such as "thread depths ±1mm USO" (Unless Specified Otherwise).

ASME Y14.5M-1994 doesn't say anything about thread depth tolerance. I'm not yet familiar with ASME Y14.5M-2009. That came out since I retired and quit consulting. It may say something. Or perhaps there is another applicable document. USA practice is to require there either be a tolerance stated on the drawing or note referring to some other applicable document that addresses the tolerance issue. That includes reference to a specific version of Y14.5M.

So if all you have on the drawing is "M4x0.7H Depth 8.00" then there is no tolerance on the depth. But note that common practice in industry recognizes the applicability of ASME thread form standards. So the M4x0.7 part is clear. Far as I know those standards don't touch on dept tolerances of threaded holes.

Here's what happens in the real world:

1. Small companies often delay developing standard drawing formats for their CAD work. ASME Y14.5M is often in the title block or a general drawing note. As companies mature they usually find that it is wise to create a standard document to cover common requirements of their parts that otherwise would have to be added to each drawing consuming drafting time and file space. The appropriate document number is then put on each drawing as a standard note. One of the common issues touched in such company standards is features of threaded holes not covered in the ASME standards. Thread depth is one.

2. Inexperienced and lazy drafters often leave thread depth tolerances off drawings. Many simply don't know how to calculate required thread depth and do the necessary tolerance studies. (Editorial comment: Often seen in today's newly minted mechanical engineers)

3. Experienced jobbing machine shops know this and follow a practice of threading deeper by a convenient amount that will guarantee a minimum depth of thread in the amount shown on the drawing but not break through at the bottom of the hole unless the drawing requires it. That is the safe practice. If break through is required common shop practice it to tap all the way through.

4. There is also the issue of the allowable size and angle of the countersink at the entrance of the threaded hole. Again not covered in the standards but necessary for a number of reasons.

5. In the absence of a standard note on the drawing or a backup design standard that is cited either in a drawing note (preferably) or buried in the purchase contract somewhere the following would be a good threaded hole callout to cover female thread linear features: M4x0.7H Depth 8.00 min, 12.00 max hole depth, CSK 5.00/5.50x40/50 degrees. Those 4 variable numbers each based on appropriate tolerance studies. Note my example may not perfectly fit requirements of Y14.5M 2009. I admit some ignorance here born of a general reluctance to invest heavily in engineering books now that I'm retired. Those ASME standards are somewhat costly.

Ed Weldon

Thanks for your help. Our designer said the thread depth is critical and he didn't add a speical tolerance for it, but general tolerane +/-0.3 list in the title block of the drawing instead. The supplier in Asia doesn't follow up this requirement and make it deeper and deeper upto 11.5mm. i think the drawing is quite clear but tolerance is not very resonable. we will add a suitable tolerance on the drawing(maybe 8.00+1/-0) and supplier agreed with this and will follow it later. But they don't accept return over thousands pcs failed parts as it are built according to ASME requirement.

The designer should prevent problems by stating why a thread depth is critical as a threaded hole is effectively a dynamic machine with various usages which is why there are no general tolerances. A typical thread application that requires an exact thread depth and possibly an exact start position for the thread lead would be a threaded hole to accept a stud in a robotic actuator. A typical application for a thread with a loose tolerance would be to accept a permanent fastener in a large object like a stamping die.

Thread depth is measured with a "go" gauge. 0.3mm is a very tight and difficult tolerance even for a 0.7 pitch tread. It likely will require expensive labor intensive sampling to control. Even 1mm will prove difficult. I would seriously question the engineering need for such tolerances. Truehart in reply 6 make an excellent points.

If your problem is arrogant and bureaucratic behavior of some entity in your organization perhaps you have a "people problem" rather than a technical problem to solve. Company quality control functionaries often annoint themselves as the "gods of quality" who can do no wrong. They force engineers and material expediters to jump through hoops to satisfy their ego drives. This can be fixed.

Ed Weldon

The thread depth has to be able to accept a 8 mm long screw. The hole depth depends on the application but must accommodate the the lead of the tap used to cut the thread. If you have a blind hole and relatively thin material then a bottoming tap must be used to prevent breakthrough. Generally speaking a machine tap is used because they are most common.

It's true that many companies have a default tolerance block on their drawing formats and you didn't say whether the drawing you have includes one. If it does, that's your answer on dimensional tolerances. When in doubt, read the drawing...then follow it. :)) Otherwise, companies may assume the machine shop will follow "general good engineering practice" even though that's not quantitatively specific.

I can think of two interpretations of your question: one is the depth of the tap drill hole and the other is the depth of the threads.

When I did mostly machine design, a general rule of thumb was that you want the thread depth to be 1 - 1.5 times the nominal thread diameter so as to develop sufficient strength in the threads to resist the tightening torque. In certain cases where available depth is limited, 0.75 D can be used in larger thread sizes but an M4 would be considered a small machine screw and 1 D minimum is what I would recommend.

Tap drill depth has no firm standard, but I used to use about 1 D of the tap drill diameter beyond the required thread depth. However, that would not apply if a bottoming tap is used to cut the threads.....then make the tap drill depth about 0.5 D beyond the minimum thread depth needed. The consideration is to make sure there is enough room for chips without having to pull the tap out often so they can be cleaned out of the hole. If too many chips accumulate in the hole, the tap will be broken.

I wasn't working in metric, but nearly all the places I worked used a tolerance of +/- 0.03 inch on two place decimal dimensions and +/- 0.015 on three place dimensions.

Drawings usually have their tolerances spelled out in a tolerance block within the title block of the dwg. I do not believe there is a standard default value that can be used. If the tolerance is not there in the title block then all dimensions should have them added.