The Good, the Bad and the Retapped

Retapping erodes profits and scuttles deadlines. Here’s how to foil undersize holes, the leading culprit behind retapping.

Here we go again. Another internally threaded part has to be reworked because the tooth space created by the tap ends up too narrow. Another undersize threaded hole. The Go thread plug gage will not enter the threaded hole at all or, at best, will only go in for one or two turns. Your first reaction is to check to see if you accidentally used the No-Go member. But, as you suspect, you are using the correct gage, and the taps received are exactly what you ordered on the requisition form.

Now you’re faced with another costly rework operation. This will mean pulling an operator off a machine to rework the part by hand, which will use up time and money. Next, you’ll have to select someone, from all the volunteers, who will call the customer and inform him that delivery will be late.

Why does this keep happening?

There are several possible causes:

• Many workpiece materials—such as titanium, aluminum, and stainless steels—have memory, or a tendency to close back in on the hole once the tap is removed. This is a common cause of undersize threaded holes, especially in thin-wall parts. The sides get pushed out from the pressure of tapping and fall back inward when the removal of the tap relieves the pressure.
• Internal cold-forming of threads is another process that is affected by material retraction, causing undersize threads. The material is pushed into the space between each tooth of the tap, creating the thread profile. Thread-forming taps are specified with higher H-limits (for inch taps) and D-limits (for metric taps) to compensate for the retraction.
• Plating a part naturally reduces the size of the threaded hole. A predetermined plating thickness can be calculated for preplate tapping. The part can then be tapped to the correct oversize condition; after plating, the part will gage to the proper class of fit.
• The most common cause of undersize holes seems to be heat treating. The part is distorted and/or scale or other residue accumulates in the threaded hole, again causing an undersize condition.

Unfortunately, the effects of material movement and heat treating are difficult to predict. When the job is first set up, the tap size is an important factor and should be established through testing and trial runs. Adding to this unpredictability is the problem of variation between material lots received. Some material will react differently from lot to lot because of a difference in chemical composition. Therefore, each lot should be evaluated for machinability and the effects of other processes to which the material will be subjected.

Given all these variables, how do you select the proper tap size? The following examples will help solve some commonly encountered problems.

Situation 1: Tapping a part with a small-diameter internal thread requiring heat treatment.
Consider a threaded hole that has to gage to a 1/4-20 UNC-2B class of fit after heat treating. Normally, we would use a GH-5 tap limit for this class of fit. The G indicates that the tap is precision ground, and the H-5 limit puts the tap size in the middle range of the Class 2B tolerance level. The proper tap size can be determined by consulting the Metal Cutting Tool Institute (MCTI) or any tap manufacturer’s catalog.

	Figure 1: Note that H-limits for taps measuring between 1" and 1 1/2" in diameter (right) have twice the tolerance of H-limits for taps smaller than 1" in diameter (left). As a result, H-limits for larger taps overlap.

However, because of the heat treatment, the GH-5 tap will produce an undersize hole. There is a 0.0005"-dia. increment between successive H-limits, and for taps 1" in diameter or smaller the H-limit is held to a 0.0005"-dia. tolerance (Figure 1). Since the zero point is basic pitch diameter, a tap with a GH-5 limit’s maximum diameter is 0.0025" over basic. And a tap is 0.002" over basic pitch diameter at the minimum GH-5 limit. In this situation, a typical response is to request a tap with a GH-7 limit, which is 0.001" larger than the GH-5 limit.

But that might not do the trick. Generally, a part requires more of a significant change than +0.001" before heat treating to fall within the class of fit after heat treating. A +0.005" (GH-11) tap is recommended in this case. The threaded part is distorted by 0.002" to 0.003" after heat treating. This change in thread size will be the same, even if we use a +0.005" oversize tap. The larger tap size will increase our chances of having a gageable part after heat treating. Knowing the constant heat-treatment distortion, we are virtually guaranteed not to have an oversize condition. That’s because the 1/4-20 UNC-2B No-Go limit is 0.2224" at the maximum; the high side of a GH-11 pitch diameter for this tap size is 0.2230". With the distortion that takes place after heat treating, we should be well under the maximum 2B limit.

Situation 2: Tapping a large internal thread in a part that requires heat treating after manufacture.
Let’s assume we have the same situation as in the previous example (including 0.002" to 0.003" distortion after heat treating), except that the thread size is 1 1/4-7 UNC-2B. As thread size increases, the amount of tolerance for the class of fit also increases. The 1/4-20 UNC-2B in the previous situation has a 0.0049" tolerance on pitch diameter. The 1 1/4-7 UNC-2B thread has a 0.0096" tolerance for the same limits.

The H-limit tolerance must be considered when selecting a tap to compensate for a process that causes undersize threads. While all H-limits are divided into 0.0005" increments, H-limits for taps greater than 1" in diameter can have tolerances of greater than 0.0010" (see Figure 1). You could conceivably use the 1 1/4-7 UNC-2B tap with a GH-4 limit and still end up with an undersize threaded hole. If this happens, you may decide only a slight change is needed and purchase the tap with a GH-5 limit. Even if both taps are within proper manufactured tolerance, the GH-5 tap could be smaller than the GH-4 tap. Even a GH-6 limit tap in this diameter might be no larger in pitch diameter than the GH-4 limit tap.

The best solution is to select a larger H-limit on the tap. If the GH-6 limit was used and the Go gage would not enter, then we know the diameter change was at least 0.002". This is still trial and error, but let’s try a GH-12 limit, which will allow for a change of 0.002" or more while still accepting the Go thread plug gage. Remember, the standard tolerance for the product thread size and class of fit is 0.0096". Therefore, you can compensate for closing-in or distortion from heat treating with a much larger H-limit and still not have to worry about an oversize thread.

Situation 3: Tapping large or small internal metric threads in a part that requires heat treating after manufacturing.
Again, we are keeping the identical conditions in place, but now the thread size is M651.0 6H. Many people are uncomfortable with metric, but we’ll all have to get used to the idea. So let’s take a moment to look at some of the terminology and designations of metric taps.

Aside from the fact that dimensions are listed in millimeters instead of inches, the metric system describes the pitch of the screw thread, rather than the threads per inch (tpi) described in the Unified System. Therefore, a 1mm pitch is just that: it indicates a distance of 1mm from the crest of one thread to the crest of an adjacent thread. For every revolution the tap makes, it has to advance 1mm.

The 6H indicates an internal thread machined to a medium tolerance—it is comparable to 2B fractional threads. To produce the proper thread size in a Class 6H fit, we must control the tap size with D-limits, the metric equivalent of H-limits. A D-5 limit should be chosen to tap an M651.0 6H thread.

	Figure 2: D-limit designations for metric taps, in this case an M6x1-6H tap.

How do D-limits affect tap size? The pitch diameter of the tap increases 0.013mm (0.0005") between successive tap-limit numbers, the same rate of increase found with H-limits. The tolerance of each D-limit number for smaller taps is also 0.013mm, or 0.0005". Therefore, the high side of a D-5 limit on a tap pitch diameter is 0.0025" over basic pitch diameter (Figure 2).

As with H-limits, D-limits increase in tolerance as thread size increases. The D-5 limit for the M6 tap has a pitch-diameter range from a high of 5.415mm to a low of 5.390mm. This is a tolerance of 0.025mm (0.00098"). Rounded off to 0.001", this is the same amount of tolerance covered by an H-4 limit for a tap over 1" in diameter.

Let’s apply this to the part we are tapping and then heat treating. Unaware of the D-limit tolerance, we use a standard tap with a D-5 limit for our M651.0 6H thread, as recommended by MCTI or the tap manufacturers’ catalogs. After we notice the extent of the thread distortion caused by heat treating, we decide to use a D-7 limit on the tap. If the D-5 tap was on the high side of the limit and the D-7 tap is on the low side of the limit, our actual change in tap size could be less than 0.0001". This would leave us with the same undersize threaded hole, and we would have no idea why it happened.

There are two extreme conditions that could occur with a large metric thread. If the thread size is an M1652.0 6H designation, we would recommend a D-8 tap limit. The actual tolerance of the D-limit for an M1652.0 6H is 0.0406mm (0.0016") This would encompass just over three H-limits for taps 1" in diameter or smaller. This wide tolerance can lead to problems. When people specify a D-limit or H-limit, they tend to think only of the high end of the tolerance. But even though the M16 tap could be in perfect manufacturing tolerance for the D-8 limit, it could actually measure the same as the maximum for a D-5 limit.

Most standard metric taps in stock in the United States are designed for a Class 6H tolerance. Consequently, when you need a larger D-limit to compensate for plating, heat treating, or material close-in, you usually have to purchase a special tap. When ordering a special, state the tap pitch diameter size you need. If you are not sure how to figure the actual pitch diameter limit for the tap, check with your supplier. If you know the D-limit needed, then request it as a GH-limit. That way, you’re putting a tighter control on the tap size, and this will enable you to determine the amount of distortion more accurately in trial runs. Make sure to be specific and write your request, so your supplier understands the tap size exactly.

The most crucial fact about H- and D-limits is that they increase in tolerance as thread size increases, causing overlapping of limits. The H-limit tolerances double when threads cross the 1" threshold, but the D-limit tolerance increase does not occur at a constant rate. As noted in the two examples, the M651.0 tap size has a tolerance on the D-limit of 0.0010", whereas the M1652.0 tap size has a tolerance on the D-limit of 0.0016. This gives us a much greater chance that different D-limits for the same tap size could overlap each other, especially on larger metric sizes.

Retapping threaded parts is costly, but it’s also avoidable. A thorough understanding of tap pitch diameter limits—both inch and metric—will decrease retapping and increase profits and on-time delivery.

About the Author
John Emond is product specialist for Greenfield Tap & Die, a division of Greenfield Industries, Greenfield, MA.