# Thread depth



## Hukshawn (Jan 15, 2017)

How do you calculate the compound depth for a given pitch? Trying to figure out the calculation is kicking my ass.


----------



## RJSakowski (Jan 15, 2017)

It depends on your compound angle.  Some time ago, I posted a chart for a 29.5º setting. http://www.hobby-machinist.com/threads/cutting-threads-depth-of-cut.37700/#post-323320.

Note that the depths are for a sharp pointed threading tool. If you have a radius, as is usually the case, that must be taken into account.


----------



## Tony Wells (Jan 16, 2017)

The pitch diameter is the more critical feature. You'll need a set of thread wires and a little patience learning to deal with them, but your threads will turn out more accurately than simply relying on the thread height (or depth as some people call it). Thread height it 1/2 (major actual - minor actual) There are instruments made for this measurement. But as long as your tool radius is correct, hitting the PD is more critical.


----------



## mikey (Jan 16, 2017)

I use Daryl Holland's method most of the time: *0.75 / TPI*. This very closely approximates the required depth of cut using a compound at 29.5. For example, 1/2-13 thread DOC = 0.75 / 13 = 0.0577. I start checking fits early so I don't over-cut.

If using the *(Dmaj - Dmin) / 2 *method, you get the depth of cut for a straight feed using the cross feed dial. If you multiply the above by *1.1433*, you get the depth of cut when using the compound. For the same 1/2-13 thread, (0.500 - 0.4056) / 2 = 0.0472. 0.0472 X 1.1433 = 0.0540".

I find the latter to be a bit more accurate but as Tony says, use the 3-wire method when fit is important. This especially applies to cutting a male thread that must fit into a part that is already threaded with a standard female thread.


----------



## Tony Wells (Jan 16, 2017)

I might add that if you have a few sizes that you find yourself cutting fairly often, it would probably be worth it to make a set of soft gages. Then, pretty much you cut your desired major, establish the proper tool radius, and cut until the gage fits. 

It gets a little involved when making ring gages, because they are smaller on the PD than the mating plug gage. I think we've touched on this before on the Forum, and maybe an in depth discussion could be started.  But basically you have to make two plug gages. One to use as a "set plug'", which has the proper PD for the ring gage, and then the working plug gage, with the high and low limits per MH. In the end, I guess you end up making 4 set plugs (explained if we do a detailed thread) and 2 working plugs, and 2 working rings to have a set. If you're really careful, you can make only 2 set plugs, but one end will actually have 2 sections with different PD's.

This is all part of why hobby machinists cut to fit nuts and mating parts. But for true interchangeability, and known good, compliant threads, you have to go to a little more trouble.


----------



## Hukshawn (Jan 16, 2017)

Wow... much more complicated than I realized... 

My wife is a bit of a university nut and loves math. I was trying to look up formulas but was having a lot of trouble. She kept me up until past midnight cause I couldn't source an answer and she was getting frustrated cause the math wasn't working. Lol. 
I found a few handy charts, but the differences between US national threads and unified (etc) has me baffled....


----------



## Hukshawn (Jan 16, 2017)

How do you use thread wires?


----------



## BGHansen (Jan 16, 2017)

I recall doing the 29.5 deg. calculation once or twice and having to go back over the thread with a triangular file to make it work.  Typically I now run the threading tool until the thread is starting to look like a "V", then start checking with the mating part if possible.  Proof in the pudding is that's where it's going to end up, so it's guaranteed to fit.  If it's a standard thread, use a hardware store nut/bolt to check your thread.

The more expensive solution is use a pitch thread micrometer like those pictured below (~$60).  They work great and as Tony mentioned above, dials you in dead nuts to the pitch diameter.  Not that it's a "best practice", but if I'm cutting multiple threads I zero out the compound after the last finish cut.  That way I'm creeping up on "0.000" on the compound instead of "0.047" or something like that.

Bruce


----------



## Hukshawn (Jan 16, 2017)

BGHansen said:


> I recall doing the 29.5 deg. calculation once or twice and having to go back over the thread with a triangular file to make it work.  Typically I now run the threading tool until the thread is starting to look like a "V", then start checking with the mating part if possible.  Proof in the pudding is that's where it's going to end up, so it's guaranteed to fit.  If it's a standard thread, use a hardware store nut/bolt to check your thread.
> 
> The more expensive solution is use a pitch thread micrometer like those pictured below (~$60).  They work great and as Tony mentioned above, dials you in dead nuts to the pitch diameter.  Not that it's a "best practice", but if I'm cutting multiple threads I zero out the compound after the last finish cut.  That way I'm creeping up on "0.000" on the compound instead of "0.047" or something like that.
> 
> ...


I've seen those and considered them. Seems easier than the wires, perhaps? The wires are much less expensive tho. Albeit, I don't know how to use them...


----------



## Hukshawn (Jan 16, 2017)

Let's make an example... an I'd like to call on your guys experience.

I've made a few barrel nuts for my spindle for various chucks and collets and thread protectors, so I have my spindle thread down pretty good... however, each time has been guess work... 
measuring the major diameter of my spindle, how much less (or more) should be the rule of thumb, if you will, for the minor diameter of the mating part, and vice versa for the opposite? Or, the minor diameter of the male part to the major of the female...

The test fit is fine. But my first attempt at my spindle thread, for example, I had started with an incorrect major diameter and to get the piece to fit I had to keep cutting until it fit, and it made a bit of a mess and I lost my shoulders, etc... 

I have an er32 collet nut in the mail arriving any day now. I have the barrel nut ready to have the nut threads cut. But it will need to be very accurate! 
How would I go about accurately transferring that female thread to my male barrel nut? What's the preferred method?


----------



## Bill Gruby (Jan 16, 2017)

Three wire thread measuring:

http://www.emte.ch/English:3-Draht-Gewindemessung.asp

 "Billy G"


----------



## mikey (Jan 16, 2017)

Hukshawn said:


> I have an er32 collet nut in the mail arriving any day now. I have the barrel nut ready to have the nut threads cut. But it will need to be very accurate!
> How would I go about accurately transferring that female thread to my male barrel nut? What's the preferred method?



Okay, I think I see where you're going here, Shawn. You have an ER-32 nut on the way and you need to know how to cut the mating male thread for it, right? You seem to be asking: 1) what dimensions to make the snout of the chuck so the nut will fit properly, 2) what the PD (pitch diameter) is and 3) how to measure the threads so you have a good fit (pitch diameter tolerances). Is that right?

An ER-32 nut has a M40-1.5 thread. The M40 part is the nominal major diameter and the 1.5 part is the pitch of the thread. Ideally, you would also have the tolerance the female thread is cut to and the maker can supply this info for you (unless its Chinese, so good luck).

1) To sort out what size to make the male blank, look here: http://www.engineersedge.com/hardware/metric-external-thread-sizes2.htm. Scroll down to the M40-1.5 row and look for 4g/6g in the next column and you'll see the min/max dimensions for the external snout. You will also find the min/max Pitch Diameters for that class of thread.

2) When you say, "But it will need to be very accurate!" you are talking about tolerance class. Again, this relates to the 4g/6g thing above. A metric class 4g is equivalent to an American class 3a fit, which is a very precise thread used when strength requirements are high. It is a precision fit that requires precision dimensions and precision thread cutting. To get a handle on what this fit stuff means, go here: http://www.katonet.com/article/science.html, and here: http://www.bluetoad.com/article/Metric+Thread+Tolerances/1799736/0/article.html. This will explain what those numbers and letters mean.

3) To cut the thread accurately, you have to be able to measure the thread accurately and the guys have given you a number of options . A thread micrometer is the best way but is also the most expensive way. A 3-wire set is the cheapest but the most tedious. Your call but the Shars thread micrometer set can be had for less than $70.00 and seems like a good way to go because it can be used for every other threading project you do.

All this info is in the Machinery's Handbook, although it takes a bit of searching to find it. And don't even think that you're the first or only one to be confused by this thread cutting stuff because you aren't. Many of the guys who do understand it were right where you are now at some point so hang in there and learn. The thing I like about you, Shawn, is that you're willing to ask ... that counts in my book.


----------



## Hukshawn (Jan 16, 2017)

Awesome write up. When I read all the articles, when I have time, it looks like it will answer a lot of questions. 
Another question tho... how do you measure, aside from the major diameter, of an internal thread? Wires or thread mic doesn't work, does it?


----------



## mikey (Jan 16, 2017)

The cheapest way to know about the dimensions of your ER nut is to ask the maker. Another way is to do as Tony suggested - make go/no-go make gauges and check for fit; this is the most practical way to go. I think I also saw something on direct measuring micrometers but there are really expensive if I recall; haven't looked at this in a very long time.

To make the gauges, you have to make at least two of them. Check the charts for the min/max dimensions and cut them.

Hopefully, someone will know of an easier way to do it.


----------



## DAT510 (Jan 16, 2017)

When I cut Threads, I mount my Dial Indicator on the Back of my Crossfeed and have the indicator measure off the back of my QCTP.   As I feed in the compound, the indicator gives me the depth without having to calculate based on angle and compound depth of feed.  I just have to remember to divide the difference between the Major and Minor Diameters by 2.  (Almost forgot on the last one )


----------



## Hukshawn (Jan 16, 2017)

Mikey, I haven't really been talking specifically about the er collet, was just using that as an example. But more so, in any future situation where I need to make a male thread to fit a female pre-made nut. 

In my mind, the only measurement I can take from a female nut is to just caliper the major diameter and calculate from there to decipher the male thread. 

What I'm trying to sort out is, when you go to make the new male thread, what do you do with that female major diameter? How much smaller do you go to make the male thread? Is there a rule of thumb? Do I just refer to the charts and use the min/max? What do you guys do?


----------



## Tony Wells (Jan 16, 2017)

There are more or less direct methods of measuring the PD of an internal thread, but the instruments to do it are not really practical for a home machinist. There is a company called Gagemaker who markets a couple of different systems, along with software to do all the calculations and also some setting standards if you are checking the lead. They have quite a variety of tools for just about any style thread. If it were me in your place, I would wait until I had the nut in hand, thoroughly clean it of all oils, then spray some cooking oil type stuff (Pam) and make a plaster cast of a little less than half the diameter. Do this with the nut standing on edge, with masking tape dams front and back. When it cures, it should come out easily, and you can get a look at the profile and if you have the right tip on a drop indicator, or a thread height gage (yes, they make such a thing) you can measure the facsimile of the thread, albeit a mirror image, so to speak. You can get a direct measurement of the Minor diameter, close enough if you have some good calipers. Then add 2x the thread height and you have indirectly come up with the Major diameter of the internal thread. You also get a look at the root radius, so you know what the crest of your male thread has to look like. Of course, there should be some clearance between the major of the external and the major of the internal. All the contact on this type of thread should be on the flank only.

I have a 50 lb box of dental plaster that sets extra fast, just for such things as looking at features that I can't get to directly. It's pretty handy also if you have an optical comparator to have a good look at the cross section of such a casting (moulage) style.


----------



## mikey (Jan 16, 2017)

You have to know what size the female/nut is. That is, you need to know if it is a 1/4-20 or a 1/2-13 nut or whatever. To do that, measure the ID of the nut and check the chart to see what the size is, then confirm the pitch or thread count with a thread gauge. Once you ID the female thread then you can look up the major diameter of the male part and cut it to the size you need. 

Many of us know what fits we need. For example, if you want to cut a 1/4-20 male thread to fit a confirmed 1/4-20 nut then you can make the male blank 0.25 minus maybe 0.005" and you'll have an okay fit in a hardware store nut. If you want a really good fit, you have to know what the female thread tolerances are and that is more involved, as we've discussed above. 

Download a chart of the common major diameters plus min/max sizes as they relate to tolerance class and put it in a folder. When you need to make a male thread, look up the size of thread you need and turn the blank to suit the fit you need. There are no shortcuts to this as far as I know. You certainly cannot infer these dimensions from measuring the ID of a female nut.


----------



## Tony Wells (Jan 16, 2017)

I can give you the dimensions for all the main thread features if you're sure of the thread.


----------



## Hukshawn (Jan 16, 2017)

Jeez. No simple solutions anywhere in machining, is there? And hell, it's also really expensive! There's a different tool for everything. 

Bare with me, guys. Believe it or not, I am learning a lot.


----------



## 4GSR (Jan 16, 2017)

Tony didn't mention, you can buy the Gagemaker software for about $125 if the price has not gone up.  You cannot duplicate the software easily, I know it very well.  But for this price, it's well worth paying the price if you deal with lots of threads like I do.  I have my own excel spread sheet that I use for most of the threads I deal with in the oilfield.  Lots of Acme and Stub Acme threads.  BTW a copy of my excel file is in the download sections of the Forum.  My program does not deal with Metric threads.  That's one nice thing about the Gagemaker, it deals with all types of metric/ISO thread forms and for $125 not a bad investment in my opinion.  Ken


----------



## Tony Wells (Jan 16, 2017)

I like the Gagemaker software, because it gives dimensions for making gages, and includes data on various pipe threads and most of all, it is not simply a list of standard threads. It uses the appropriate formulas to derive the dimensions from what you give it. You want to cut a 1.900-32? It will give you all the data. And if you don't have the recommended wire, you can alter that and it will provide MOW numbers for the wires you do have, provided you accept the fact that they don't hit the pitch line. And of course, if your choice is too small it won't stand out over the major so you can't really measure it very handily. I recommend it too, and have known the main distributor for about 20 years I guess....other than a friend, he's been a good vendor for me.

Although it won't do RSC or API style threads, unless the newer version does, that's the only drawback I can see. The company also offers tools for measuring those threads, but I believe it is in a different software package, although I'm not certain about that.

Their whole claim is that you do not need solid plug and ring gages. You can inspect each thread element independently and make a determination of acceptance or rejection. If that is true, and I won't say it is or isn't, even though their system is expensive, so is a complete set of solid gages.  Even more expensive, by a long shot.


----------



## pstemari (Jan 17, 2017)

Hukshawn said:


> How do you calculate the compound depth for a given pitch? Trying to figure out the calculation is kicking my ass.



For a sixty degree UN thread, it's 5/8 * the pitch.  E.g. for a 20 TPI thread, the pitch is 0.050" inches and the compound travel is 0.03125.

It's not a particularly useful measure, though, since any error in the width of the flat on the end of the thread tool will get reflected in the pitch diameter.  Better to measure the PD using a thread mic or thread wires.



Tony Wells said:


> ...Their whole claim is that you do not need solid plug and ring gages. You can inspect each thread element independently and make a determination of acceptance or rejection...



Simple Go/No-go plug and ring gages can't measure all of the thread elements, although arguably they measure the ones that matter. For example, if the pitch diameter of an external thread, is ok, but the root is cut too deep, a simple no-go gage won't fit. Same is true of a internal thread whose minor diameter is too large. You'd need three no-go gages to test the usual thread parameters.


----------



## BGHansen (Jan 17, 2017)

DAT510 said:


> When I cut Threads, I mount my Dial Indicator on the Back of my Crossfeed and have the indicator measure off the back of my QCTP.   As I feed in the compound, the indicator gives me the depth without having to calculate based on angle and compound depth of feed.  I just have to remember to divide the difference between the Major and Minor Diameters by 2.  (Almost forgot on the last one )
> View attachment 155936


Great idea, wish I'd have thought of that!

Bruce


----------



## mikey (Jan 22, 2017)

Hukshawn said:


> In my mind, the only measurement I can take from a female nut is to just caliper the major diameter and calculate from there to decipher the male thread.
> 
> What I'm trying to sort out is, when you go to make the new male thread, what do you do with that female major diameter? How much smaller do you go to make the male thread? Is there a rule of thumb? Do I just refer to the charts and use the min/max? What do you guys do?



Shawn, I just re-read my responses to this thread and I recalled that I saw something about how to figure out the size of a male nominal OD when only the female part is known. It bugged me that I didn't answer you accurately so I went looking for it and found it: http://mdmetric.com/tech/tict2011.htm#cht8

I read this years ago but forgot about it. Don't laugh; when you get to be my age you'll be happy just to remember to get out of bed in the morning. Anyway, scroll down to the bottom of the text section and you'll see Chart  VII: HOW TO CALCULATE THE APPROXIMATE NOMINAL MAJOR DIAMETER (O.D.) OF THE METRIC MALE (EXTERNAL) THREAD WHEN ONLY THE FEMALE (INTERNAL) METRIC THREAD IS AVAILABLE FOR MEASUREMENT.

Take a look at the instructions and you'll see how to size the male part. This is for a metric thread and I don't know if the Factor Value, R, applies to imperial threads. I have sent an email to Maryland Metrics about this and will put their answer in this thread if they ever respond. 

So, from the ID and pitch of a female threaded part, you can determine the nominal OD of the mating male part. You then cut the external threads on the male part using the tolerance specs you choose and the parts should fit. Hope this helps.


----------



## Hukshawn (Jan 22, 2017)

Now there we go... 
you said before, the collet cap will likely be metric anyways, so this should help with this project.... whenever that damn thing shows up...


----------



## KBeitz (Nov 22, 2018)

You would thing that someone would make a Dial Indicator that would read half 
for things like this...I would think it would be a HOT selling item...


----------



## pstemari (Nov 22, 2018)

The ideal major/minor diameter have the same proportions for ISO metric and UN inch threads: major diameter = minor diameter + 2 × ⅝ × (the sharp v height), where the sharp v height = (cos 60°) × ½ × pitch.

That said, those instructions will only get you sort of close. The minor diameter of an internal thread varies depending on the amount of thread engagement, and frequently the minor diameter is drilled oversize to make tapping easier.

Going back to the OP's question, the depth on the compound would ideally be ⅝ × pitch = 0.625/TPI, but that typical isn't a useful measurement since it depends on the tip of the tool having a flat of exactly ¼ × pitch. If the flat is narrower, then the cut must be that much deeper. If the tool is perfectly sharp, then you would go in ¾ × pitch = 0.75/TPI.


----------

