Threadmilling questions

Hi; I wanted to make a big aluminum plate with threaded holes in it to use with bolts to hold my stock down (the sticky tape works, but I’m not a huge fan of it - it seems so… inexact, and messy). What I have in mind is something kind of close to what @jonniemac posted here.

I have no experience with machining, so I don’t know what I’m doing, and was hoping somebody could point me in the right direction.

From what I understand, the correct procedure is to drill the inner diameter hole first, and then switch to a threadmill and carve out the threads.

  1. Is that correct?

  2. How much do I need to care about the internal diameter of the hole that I drill first? I found this which describes, for example on M5x0.8 threads, an interior diameter hole of 4.134-4.334mm. Do I actually need to make a 4.125mm hole, or will the threadmill take off the rest of the material if I drill only a 4mm hole? If I have to make a 4.125mm hole, would the correct way to do that be to drill out a 4mm hole with a drill mill and then expand it out with a regular flat mill?

  3. I assume with the nomad, I’d need to thread mill from the bottom up (because if I went top to bottom, the hole would fill with chips before I got to the bottom). Or does the helical flute manage to eject the chips out of the hole somehow? If I go from the bottom up, then all the threads will get cut at once if I get a normal threadmill like this. Does the nomad have enough horsepower and stability to cut a whole bunch of threads at once with one of these? Or do I need to get something that will only do one thread at a time, like these? Or maybe one of the ones with 3 pitches of threads? Would I be able to cut the entire depth of the thread in one pass, or would I probably have to do several passes at increasing diameters? (This would be in aluminum).

  4. How does one size a threadmill? If I understand right, a threadmill can mill any size thread from some minimum size and up as long as the pitch is the same, correct? If I want to mill an M5 thread, does that mean I get an M5 threadmill (like, has the M5 threadmill been sized down so that it can mill an M5 thread?) or do I have to size down, and if I have to size down, by how much?

  5. Anybody have a favorite supplier of these? Or endmills in general?

  6. Not 100% directly related to threadmilling, but: this aluminum plate I want to make - could I use it to replace the aluminum base table that comes with the nomad itself, or would that be a bad idea?

  7. Anybody have the specs for that base table? The location and diameter/pitch of the threads that we use to attach the spoilboard to the table, but also the location/size of the holes used to attach the table to whatever’s moving along the rails underneath?

Thanks! Sorry for the battery of questions.

Fair warning, I have not used a thread mill yet, but I will and I have been doing my reading. I can’'t wait to hear how others do before I try it myself. On with my thoughts:

My two big concerns are chip removal and rigidity of the mill. Small errors make for lousy threaded fastener fit. For chip removal I am thinking about using compressed air to blow chips out of the hole. I can not see the thread mill clearing chips from the hole. We will see.

The more material you remove at one pass the more power required and the more force the mill will need to resist. I’m planning on starting with a single profile mill and seeing how it goes.

Thread mills are not cheap! There is a vendor on Ebay who seems to have very reasonable prices and good feedback. I will probably buy one of those and see what happens. Search " SINGLE PITCH THREAD MILL"

I saw this guide to using a thread mill:

A quick read on helical interpolation can be found here:
Lots of good orientation for the newbie on this site.

I want to remove as much stock as I can before hitting a hole with the thread mill. A drill or end mill will be much better at material removal than a thread mill. We have a trade off between using more tools to get better cutting performance and the time it takes to swap the tools. If we use a drill to clear out the hole most of the way, then an end mill to open up the hole to exactly the right diameter then the thread mill to put in the threads we will get the most efficient material removal but we will be spending a lot of time swapping tools. Swapping time would be less of an issue if we are making a tooling plate for our mill with a jillion threaded holes. The first time will be about learning, efficient production can come later.

Anyone out there tried this yet on any kind of equipment?

1 Like

Hey, so do you know if there’s a maximum size threadmill cutting diameter to cut a particular size internal thread (other than obviously just sizing it so it’ll fit down the minor diameter hole that you pre drill)?

It seems like the relationship between the cutting diameter of the threadmill and the size of diameter of the hole you’re trying to mill would slightly change the thread profile, right?

Does this seem like a reasonable plan to mill M5x.8 screw holes?: According to various sources (like this for example), the minor diameter I want to drill is 4.20mm, which is .165 inches. So I was going to use this 1/8 diameter drill mill to drill the hole first, then widen with a ball or flat mill, and then does this thread mill look like the right size threadmill? .138" cutting diameter should fit in the .165" diameter hole. Thread range says 24-56, (and I believe .8 metric pitch is really close to 32, so that should be in range).

Just want a sanity check before I spend $60(!) on a threadmill!

My tap and drill chart says to drill with a number 19 drill for a M5x0.8 thread. That’s .1660" inches or 4.2164 millimeters. The hole size for metric thread cutting is typically the diameter minus the pitch so … 5 minus 0.8 = 4.2.

Side note: I don’t know what cam software you’re using but if it’s Fusion360 CAM, the latest update wiped out the “Form Mill” cutting tool because it didn’t work correctly. You have no way to define that type of thread mill at the moment. Not sure if there is a workaround but I haven’t dug very deeply into the problem.

Thanks - yeah, I figured I’d either purchase a perfectly sized drill, or widen out a smaller hole with another endmill. I suppose if I end up wanting to make a bunch of M5 holes it makes sense to get the right size drill. Although I actually don’t have any intuition on how much of a speed difference we’re talking about.

Regarding Fusion360: I did a bunch of poking around on the fusion forums earlier and it seems like you don’t actually need to define the thread mill shape (in the form mill) - you can just use a “flat mill” tool and set the cutting diameter to the cutting diameter of the threadmill and it will generate the right toolpath if you ask it to generate a thread milling operation with it.

Faster to drill than interpolate a bunch of holes! And if you’re already planning to drill, might as well do it to final size.

I’ll test out that Fusion workflow and see what the tool path looks like … that’s the trick I used to do the CAM for this type of thread mill and it simulated correctly. Haven’t run it on the mill yet though.

So one of the reasons I was going to drill a 1/8" (3.175mm) hole and then widen it is I couldn’t find any 4.2mm (#19) drill mills. Does such a thing exist, or is it ok to just stick a regular drill bit into the mill? I assume the mills are running at a much, much higher rpm than most drill bits would like, though, right?

Do you have a source of 4.2mm (#19) drill mills that you’d recommend?

You should be able to drill, just remember that you’ll need the proper collet to hold the drill bit. I picked up a cheap set of ER11 collets off Amazon. Looks like you’ll want a 4.5mm collet which holds a range of .157 to .177, you can get them by size at Maritool.

I get all of my carbide drill bits from Lakeshore Carbide. I’d recommend the “screw” length as long as it will go all the way through the hole you’re drilling. They are shorter and a little more rigid than the “jobber” length. Here’s the page and you want to select 19 in the size dropdown.

Search google for a drill and tap chart, they’re very handy … I got a nice plastic one from Maritool when I placed an order with them. I’ll make it even easier, here’s a link to one.

1 Like

Thanks - I was looking at those but from what I understand (which is not very much) I’m not supposed to use tialn on aluminum and they don’t have uncoated drill bits. Maybe one of these

Thanks for the er11 collet links. Looks like a I need a 4.5mm collet for the drill bit and a 5mm (or 3/16") collet for the 3/16" shank threadmill…

BTW, regarding Fusion360, last time I took a look at it, the toolpath for the thread milling operation looked pretty good in the simulation (and you could make it take multiple passes to slowly increase the diameter of the cut).

I’m using the TiAln coated carbide drill bits in aluminum. Basically, from what I’ve read, steel coatings are fine for aluminum but aluminum coatings like ZrN or DLC aren’t good for steel. You can go down in hardness of material but shouldn’t go up. Any number 19 drill bit should be fine … split points help to prevent the tip from walking. I went with carbide to eliminate the spot drilling step … “If you use a carbide drill, or a screw machine length drill, spotting is typically not needed.” from CNCCookbook.

I found this YouTube on thread milling:

Time to buy a thread mill and see how this works with Fusion 360.