Help with Thread Milling Math

So I’m working on making some brass branding irons but I’m still in the design phase (and consequently the tool buying phase). The general idea is that I will be milling some holes with 1/4-20 thread into the back of the irons to accept the same spec threaded steel rod for a handle. I know 1/4-20 is small for that purpose but these irons are relatively small as well.

I’m thinking of buying a 1/4" single form thread mill for this purpose, so that I can use it potentially for more than just 1/4-20 threads. If I understand correctly for an internal threaded hole, I want to drill / mill the hole to the minor diameter of the thread spec. For 1/4-20 with a 2B class of thread fit, I would want to drill or mill to .1887" which is the minor diameter. I would think I would use a #12 (.189") but a chart tells me to use a #7 (.201") for brass. So which diameter hole is the correct size to drill or mill to?
The chart: http://www.engineershandbook.com/Tables/taphole.htm

Then if I am using Fusion to design the hole and toolpath, what size hole should I design? Major diameter (.25")? Minor diameter? The drill size (whatever the correct answer is from above)? If I understand, my thread pitch is .05" (or 1"/20 TPI) but would I use a pitch diameter offset of .0613" (Major diameter of .25" - minor of .1887") or would it be 0? I’m getting confused and need help learning here.

From older threads, I have seen @mbellon and @RichCournoyer provide good thread milling advice, so I would appreciate their input as well if they are around.

2 Likes

I’m going to be a giant wet blanket here :slight_smile: I’ve gone down the path of cutting and tapping my own threads manually, both on a cnc and manually with a cutter and a metal lathe. It’s really cool, and might be considered fun, but it is stupidly time consuming and easy to botch. Specifically since you’re looking at doing 1/4-20 threads.
I would grab a tap and die in 1/4-20 and just use those. Your results will be perfect and it will save enormous amounts of time in the long run.

Or do it by hand and enjoy it :-D! Your call!

2 Likes

I do appreciate the advice, but this is definitely not for production, this is for my own learning. I do own a tap and die set, so you are correct, I can easily tap the holes by hand and be happy. But I want to learn. I’m probably one of those weirdos who isn’t happy when something works, I want to know why it works. So I know how to drill and tap a 1/4" hole but I want to know more. I’m sure you understand.

3 Likes

Power to you man, enjoy the process!!!

I’ve referenced this a number of times, maybe it’ll help you too; https://littlemachineshop.com/reference/tapdrill.php

1 Like

The difference in size is due both the required clearance in the thread to prevent binding/interference on assembly and the reduction in load when threading with a tap. For steel, typical is a 60% thread, or a little more, and 75% or so for red metals and aluminum in most cases, where a 100% thread is the theoretical profile (not the sharp profile, but the to-the-standard profile with appropriate crest and root truncation) Minimal strength is lost, but the load on the threading tool is greatly reduced, especially when tapping-- taps break easily and are a pain to remove.

The additional root clearance also reduces interference due to less than perfect thread form, making fitup easier and keeping face-to-face contact for the threads.

Most charts specify the percent thread they are sized for, and most common is 75%.

So @enl_public, if I understand correctly from the chart that I posted (and same one on different site from @Adam_Xett), the 75% for Brass at 1/4-20 indicates the recommended thread engagement so drilling with a #7 (.201") gives you the clearance for assembly as opposed to using the minimum diameter of .1887". So when creating my toolpath, I would want my thread mill to cut a .049" offset (.25" - .201") from the wall of my hole which gives me that depth of thread. Or would I still want to cut an offset of .0613" (.25" - .1887") from the wall of the hole with a diameter of .201"?

As @enl_public said, the most common percent thread is 75% as this is what would be used for the softer metals. Harder metals, 60% is more typical. The #7 is way to go. Follow what @enl_public advises.

I usually don’t thread mill, I formally tap… but this is because I have a reversible spindle and G-code support for the wonderful tapping functions.

mark

@mbellon okay thank you. Can you help me with the other questions regarding essentially how deep my threads should be cut from that .201" (#7) diameter hole?

How deep depends on what you’re doing - through hole or blind (only so far down).

Through hole is easy - make sure you go all the way through and a bit more so the threads go all the way to the bottom. If you’ve got a spoiler board, make sure it is thick enough (DANGER! DANGER!) and drill into the spoiler board. I usually drill and thread about 0.1" extra… but this is with my taps and such.

Blind is a bit more complex. You need to know how far you need the threads. They you need to drill that much PLUS enough so that the tap/threadMill can get to the depth you need. If you’re drilling, how to do this is a bit different than end milling… the drill has to go further in (think of the front of a drill vs. a square end mill).

With a drill, one need to go the depth of the cone at the front of the drill plus a bit more to ensure things (clean hole to the necessary depth). One need the depth of the “cone” at the front of the drill plus “a bit” (0.020").

With an end mill, there is no “cone”.

In both cases, you need to clear the tap/thread mill. In the worst case, I pull out a calipers and check, then add some “slop”.

mark

1 Like

Evan,

Sorry but I’m not reading all the answers below due to time constraints, but let me tell you what I recommend:

  1. Minor diameter hole should be 0.201–0.205 in.³

  2. if you have that thread mailed on your machine I recommend doing what I did for the beginner, is to make your own Threadmill from an old quarter 20 tap.

2 Likes

@mbellon thanks for the replies so far. Learning is occurring! I may have misspoken earlier, when I said “deep”. I’m trying to figure out how far radially I need to cut the threads. So how “deep” would be how far from the drilled hole wall I need to cut into the wall (If my hole is aligned with the Z-axis, I’m talking about distances in the X-Y plane) to give the proper space for the major diameter on the bolt. I think I need to ultimately be at grooves inside that hole that would be at least a .25" diameter, but I’m thinking I need to go further than that to allow for some tolerance, just in terms of machine precision.

The actual depth of cut depends on a number of things, some of which are:

Desired fit: How loose do you want the threads? Easy running fit, like general purpose nut and bot from the home center? Reasonable fit, but free running? Minimal play, like threads used for precise location, as in a micrometer? Mild interference.

Size and geometry of the cutter: The cutter will have some tolerance specified, and there will be a stack of runouts and size errors that determine that actual cut. If your spindle is true and the feed axes don’t have significant backlash or play, the biggest uncertainties are the actual machine feed (is a 1.000mm theoretical actually 1.000mm on the machine? Are the axes matched?) and the actual tool size ad geometry. You need to specify the actual tool size for Fusion (and any other CAM system). If you do, and select thread milling, I believe the CAM engine will follow the thread size and fit spec from your CAD model (I will try this and revise if I am wrong here, but it will take a little while. I am presuming that it is the same as Inventor in this respect)

The general model for the tool should be available from the supplier. The exact size may or may not be, and you will want to cut a few threads on test parts, measure them, and tune the tool dimension to match the actual cut. I would do this ion an external thread unless you happen to have thread plug gauges handy. You can measure the external over wires using a caliper and be within 0.05mm (0.002"), which is more than good enough for a 1/4" thread. If the thread pitch diameter is 0.10mm oversize on the external thread, then your tool is 0.10mm smaller than your specified, so you adjust the diameter up. Try again. In my experience, two iterations is generally sufficient, and the third cut will come in on size, to the limits of the measurments.

EDIT: just tried it. Fusion wants the hole pilot first, then thread the hole. You specify the pilot. When you thread the hole, select nominal thread and fit class, specify the thread mill in tool selection (there are none in the samples… select your library, new tool, thread mill, and specify the pitch and OD of the tool) Fusion will generate the tool path for the proper fit. Again, I would run a few test cases to insure the size is correct. In fact, I would run test cases for different fit classes to see the difference (1B is loosest internal, 3B is closest internal, in the US. 1A through 3A are the corresponding external classes)

EvanDay,

I’m currently working on making a production operation to tap 1/4-20 holes in 3/4 in HDPE so not brass, your mileage will definitely vary.

I’m currently testing my approach on a Nomad before I move it to my Shapeoko. I don’t have my Shapeoko as dialed in yet so I wanted to use the Nomad first to test my assumptions.

My current approach (being refined), is to drill my holes first. I drill to -1 mm from the bottom. I’m making a through hole in my material with a bit extra to poke the bit through. I’m experimenting with a number of bit sizes ranging from .1875 to .196. I want to remove the max amount of material with the drill but still have enough to do a good thread mill. I can’t recall why i didn’t go with a #7 diameter hole (that may still happen if needed). The biggest challenge I am having with the drill bit on the material is birds nests. I’m drilling 117 holes at once and I have issues around the 60th hole. I’m not pecking so I will try that next even though it will slow my cycle time. I may end up breaking the job up.

I strongly recommend testing on a lighter material like hdpe or wood prior to doing this on brass. Threadmills can be a bit pricey and I think the S3 could snap a 1/4-20 easily.

I don’t model my threads in Fusion 360 so I’m not sure how to handle it that way.

For my 1/4-20 threads, I use the following :
Tool: Lakeshore carbide threadmill
cutting diameter .1875
body length 2.5 in
flute length .5 inche
Flute count : 3
tooth count : 10 (this isn’t true, I have more but I want to make sure I hit some threads repeatedly)
shaft .1875
shoulder .75 in

In your case, with a single form, I would likely use multiple passes and such. In my case, I have so many to cut, I am trying to get it done in one hit.

Modeling-wise, I chose a 5mm hole (.1968 in) for my hole diameter. Similar to a #9 bit. I do a Thread operation with a top height of 1 mm from top, a bottom height of -12.7 mm from top (aka .5 in) . A thread pitch of 1.27 mm (aka .05in) and a radial stock to leave of -.93mm. In Leads and Transitions, I lead to center just to be safe.

For me, all the fine tuning is around the stock to leave. I could adjust my modeled hole size but really, I just need it to not reject my tool in the CAM op for being too small a hole. I’m controlling the actual hole size with my drill op and the bolt fitment with my stock to leave param. The smallest changes in radial stock to leave lead to huge feel differences when testing the fit. That’s why I will really need to dial in my S3 in order to make sure i have a good repeatable fit on the tapped holes and I’m not stressing my threadmill too much.

I start with multiple drilled holes and then I slowly change the radial stock parameter while testing the fit in test material.

I’ll let you know if I ever get a good recipe on the S3. It will only apply to HDPE but it might help.

good luck!

1 Like

@Jotham, Thank you for the excellent advice. I’ve been off my machine for several weeks now due to work, but my supplies for this project should be here tomorrow. I didn’t get a chance to buy a single form mill yet, but I have been playing around in Fusion to try to get the CAM correct. Its a shame that Fusion still can’t model a single form thread mill properly, but now that they introduced the Form Tool function in a recent update, I may try to set one up that way. In the meantime, I think I am going to use the SO3 to drill the holes I need threaded (that way they are straight, or at least straighter than my calibrated eyeball will allow), and I will thread these by hand. But, I plan on testing a single form thread mill out in the near future on some of the leftover brass scraps I will end up with.

Yeah, please let us know how your experiments pan out. I finally got everything working well on the Nomad and am working on porting my experience to the S3. The interesting challenges I hit with HDPE was not in the area of accuracy but rather getting the right speeds and feeds to avoid clogging the bits. If my drill bit was too aggressive, it would create a melted birds nest of plastic and eventually stall out. The same problem happened with the thread mill, to the point that I had to do a retract to make sure the mill was cool enough. My S3 has a vacuum system which I hope will allow me to push the envelope a bit without melting the HDPE onto the tool. I would imagine there would be similar considerations with brass and making sure chips are cleared so they don’t bond to the cutting surface.