Thread cutting dilema?

There are thread charts that list the outer and inner diameters for internal and external threads in the range of classes from loose fitting to very tight tolerances.

Sent from my H3123 using Tapatalk
 
Screw thread micrometers will only measure a limited number of thread leads per anvil set and will require a standard for setting them.
Wires and plain micrometers will measure any lead also Whitworth and Acme/Metric Trap threads and gears and splines. They are far more versatile unless you are in a production setting.
 
GrayTech said:
There are thread charts that list the outer and inner diameters for internal and external threads in the range of classes from loose fitting to very tight tolerances.

Sent from my H3123 using Tapatalk
Click to expand...
The IMPORTANT dimension is the Pitch Diameter, you will notice that it always has the smallest variance between Min. and Max.
All straight thread gauges are marked with the PD
For example https://www.threadcheck.com/thread-ring-gages-unified-inch/
 
C-Bag said:
So where do you find the "blank size"? A lot of what keeps me from finding info is I don't even know what it's called.
Click to expand...

Oh, trust me, I remember the beginnings and I totally understand what you're saying.

Okay, lets make things as simple as we can. The first thing to do is to sort out the nomenclature of threads. This is a good but brief summary that will help in our discussion: http://portal.ku.edu.tr/~cbasdogan/Courses/MDesign/course_notes/fasteners.pdf

I won't go through the different types of threads (UNF, UNC, etc) but I want to focus you in on the fit classes, 1-3. Loose is class 1, normal is class 2 - this is the typical hardware store fit, and class 3 is a fine, high tolerance fit. You will rarely go for a class 1, usually go for a class 2 and sometimes go for a class 3. Note that this class stuff applies to both internal and external threads. As a hobby guy, you can use whatever you wish and this is especially true when both internal and external threads are made by you; you can cut one and make the other one to fit.

The problem comes when you have to cut a thread to fit an existing part that you do not have in front of you or that is difficult to reach, or that you wish to have a specific fit for some reason. Then you need to cut the thread to some standard that will guarantee a fit. That is when you really need thread wires or a thread mic, and you need to know what those standards are. Fortunately, this is not difficult if you have a good chart. I am attaching the best chart I've ever seen for this kind of thing.

Let's use a common thread as an example, say 1/4-20. Here is an excerpt from the chart:

screen shot.PNG

Find 1/4-20 in the Thread Designation column and decide what class thread you want. Say we want a class 3 external male thread, or class 3A. Now look under Major Diameter and you'll see two figures, 0.25 and 0.2419. That is the size range your blank must be to cut a class 3 external thread so turn the work piece down until it falls somewhere inside this range, then chamfer the nose of the work piece at about 30 degrees for a length of about 1 to 1-1/2 threads. Similarly, if you wanted a class 2 fit, note the size range and cut the work to that size.

It is wise to also cut a thread relief at the end of your thread. This allows your tool to run off into that space and leave a clean thread end. There are specs for this sort of thing but I usually just make it about two to three threads wide and about 0.003" - 0.005" deeper than the minor diameter. This will not significantly impact on strength. EDIT: use your parting tool to cut the thread relief. I use a P1-N blade that is only 0.040" wide; this allows me to cut as many side-by-side slices to get the thread relief as wide as I need it to be.

Now you have a blank that is the right size, is chamfered properly and has a thread relief. To be sure your gearing is correct, make a single pass at about a 0.001" depth of cut and use your thread pitch gauge to make sure the pattern matches the gauge. If it does then your gearing is okay and you can proceed to cut the thread. What should be entering your mind now is ... how deep do I need to go to cut this thread?

There are formulas for this kind of thing. The simplest one I know is from Darrel Holland of API: 0.750/TPI. In our example, 0.750/20 = 0.0375". So, you would need to feed in 0.0375" when feeding in with the cross slide only. If you prefer to use the compound set at 29.5 degrees then multiply the above number by 1.143 and use that depth. Keep in mind that these are estimates; you need to stop your cuts about 0.005" or more before you hit the calculated depth and check the fit with your wires or thread mic.

EDIT: I suppose I should tell you how to stage your cuts. When you screw cut a thread, the deeper you are, the greater the cutting forces become. This is because more and more of the flank of the cutting tool is in contact with the work piece. This is especially true when feeding straight in with the cross slide so you don't want to try and cut the entire thread in a few passes; you should stage your cuts so that the deeper you go, the shallower you set your depth of cut. Personally, on threads below 3/8", I make the first pass a scratch pass of about 0.001" deep and check to be sure my gearing is okay. If it is, then I make a 0.009" deep pass to debulk the thread. Then I reduce the depth of cut to 0.005" deep for the next two passes, then 0.004 X two passes, then 0.002" deep X two passes and then 0.001" until I am at final depth. I've tried all kinds of patterns but on smaller threads under 3/8" I have found that going lighter gives me less deflection so my thread form is better and definitely more accurate. Lots of guys use deeper cuts and that's fine if it works for you. I prefer to go slower so I hit the size I want dead on. For me, the smaller the thread, the lighter I make my passes. When cutting threads greater than 3/8", I will make several passes at 0.009 - 0.010 to debulk, then step down as above. It takes longer to thread like this but I'm usually in no hurry; I would much rather go slow than have to make the piece all over again.

Note that the next two chart columns fall under Pitch Diameter and again, this is a range. The idea is to check the pitch diameter of your thread until it falls inside this range and that will give you the fit for the class of thread you're cutting. If using wires, you have to do some calculations. If using a thread mic then the reading is direct. Cut until you're inside the desired range and you're done.

So, what about estimating depth of cut for metric thread? They use pitch, not tpi. Just use the Newmann Tools chart below and plug the conversion into the Holland formula and it works fine.

See, not hard, right? If you use a really good HSS tool then hitting these numbers is much easier. Carbide inserts also work but you will find taking micro cuts to be less precise. On large threads this isn't usually a problem but when cutting smaller threads, it can be.

Cutting internal threads is much more difficult to do, especially when cutting to a class 3 fit. The best option is to make a plug gauge to specs then cut the internal thread to fit. I use solid carbide threading tools for small holes and a solid carbide inserted bar for larger holes. The reason for using carbide shanked tools is accuracy. When you're threading in a relatively deep hole, tangential and radial cutting forces are very high and you need to reduce deflection as much as possible; carbide will do that for you. For small holes, 3/16" and under, I use Micro 100 solid carbide internal threading bars; they are extremely accurate and stay sharp for a long time. Plus, they are easily sharpened with a diamond stone when needed (just hit the flat on top).

When you cut threads with a good HSS tool, it will usually leave a good finish and just require a quick pass with a steel or brass brush. Carbide tools sometimes need a quick pass with a fine file to clean up.

Hope that makes it easier for you guys. Thread cutting is not difficult; you just need to practice.
 

Attachments

  • American-Light-Screw-Socket-Thread-Specification-Sheet.pdf
    165.1 KB · Views: 21
  • TPI to MM conversion chart1.pdf
    49.3 KB · Views: 6
Last edited:
Made a few edits to my post above.
 
Bullseye Mike, especially the first link. For some reason I can't open the last two attachments.
 
Yeah, I wish they still had the Starrett no. 392 fishtail holder. I think they quit making them. That would be so handy I think I'll have to make one. Use a fishtail once and you'll wish you had one too.....
 
mikey said:
EDIT: I suppose I should tell you how to stage your cuts. When you screw cut a thread, the deeper you are, the greater the cutting forces become. This is because more and more of the flank of the cutting tool is in contact with the work piece. This is especially true when feeding straight in with the cross slide so you don't want to try and cut the entire thread in a few passes; you should stage your cuts so that the deeper you go, the shallower you set your depth of cut.
Click to expand...

I think Cat Stevens summed it up best (or Sheryl Crow for you youngsters):

"The first cut is the deepest,
baby I know,
the first cut is the deepest"
 
You must log in or register to reply here.
Back
Top