Tips/Tools for machining large diameter threads on mill

[Elemental_Garage]

Hello all,

I'm in the process of designing/milling a coolant overflow reservoir for an auto project. I have it in 4 pieces; the cap with external threads, a weld-ring with internal threads (this will get welded to next part), the main body which will just be tubing, and the bottom that will be tapped for a drain plug.

The threads I'm making at 2 3/8"-12. For my test cut I used the largest single-form thread mill I had, which is designed for a 1/2 thread. I see that Harvey has single-points going up to 1", but nothing beyond that. My test cap and weld ring actually came out better than I thought, however about half-way through threading it becomes overly tight. I think I made the tolerances too tight. I was limited in the PDO I could use to make the threads deep because I'd run into the tool body. I made the PDO of the internal threads a bit deeper than external, but likely not deep enough.

I'm curious though if anyone has tips on doing these larger threads where you're making both the internal/external threads. I acknowledge the tool I am using wouldn't likely make threads that would engage with a standard 2 3/8"-12 piece due to thread depth, but I also know I can't spend $200 multiple times over for each size and need to find something that will work well in these 2-3" range of making threads, if that makes sense.

Any tips/tricks/points for both process and tooling. I'm using Fusion. I'm also wondering if I had my speeds/feeds right to make clean cuts. I programmed it for the recommended tooth load (0.00068), but I can't get to the SFM recommended with my 6,000 RPM limit.

Here is the test part:

 

[rklopp]

The thread pitch is what counts, not the diameter. So if your thread mill could cut, say 1/2-12 threads, it should be able to cut 2 3/8-12 threads, too. Is your cutter rated to do 12-pitch threads? If so, I would think just putting on a little negative wear offset would loosen up the fit. On the other head, if the thread mill is limited to 1/2-13, then you may well be running the tool neck into the work, especially if you're hitting a burr or you have chips caught between the shank and work.

 

[Elemental_Garage]

The thread pitch is what counts, not the diameter. So if your thread mill could cut, say 1/2-12 threads, it should be able to cut 2 3/8-12 threads, too. Is your cutter rated to do 12-pitch threads? If so, I would think just putting on a little negative wear offset would loosen up the fit. On the other head, if the thread mill is limited to 1/2-13, then you may well be running the tool neck into the work, especially if you're hitting a burr or you have chips caught between the shank and work.

Here is the tool I have: https://www.harveytool.com/products/tool-details-901270-c3

 

[rklopp]

Per Harvey, the max thread height you can generate with that cutter is 0.069" before the shank rubs. CNC Machinist Calc Pro gives a thread height of 0.0722" for 2.375-12. Therefore you will need to make the internal thread minor diameter a little bigger and the external thread major diameter a little smaller if you're going to make it with that cutter. Given the application, I don't see an issue tweaking those diameters by, say, 0.010". It likely will take less tweaking, given that the parts already go together partway.

 

[dodgin]

We use and love the Ingersoll Rapid Thread family of tooling. If I get what you're saying is that you don't want to drop $200 every time you need to mill a thread, something along those lines will come in handy. Just buy a body or a few if that's what you need and you'll easily be able to find the correct pitch insert for whatever your project is. Bonus that Ingersoll tooling is interchangeable with Iscar and also Tungaloy I believe...you can usually always find what you need in stock from one of those outfits.

 

[Elemental_Garage]

Per Harvey, the max thread height you can generate with that cutter is 0.069" before the shank rubs. CNC Machinist Calc Pro gives a thread height of 0.0722" for 2.375-12. Therefore you will need to make the internal thread minor diameter a little bigger and the external thread major diameter a little smaller if you're going to make it with that cutter. Given the application, I don't see an issue tweaking those diameters by, say, 0.010". It likely will take less tweaking, given that the parts already go together partway.

Thanks for that info. In the context of Fusion, would that height be the same as the pitch diameter offset?

 

[Elemental_Garage]

We use and love the Ingersoll Rapid Thread family of tooling. If I get what you're saying is that you don't want to drop $200 every time you need to mill a thread, something along those lines will come in handy. Just buy a body or a few if that's what you need and you'll easily be able to find the correct pitch insert for whatever your project is. Bonus that Ingersoll tooling is interchangeable with Iscar and also Tungaloy I believe...you can usually always find what you need in stock from one of those outfits.

Thank you! I will look into these!

 

[rklopp]

Thanks for that info. In the context of Fusion, would that height be the same as the pitch diameter offset? View attachment 407792

That sounds right. If the numbers in the box are right, your cutter should reach since the depth appears to be 0.042". When I do threads in Fusion with single-profile cutters, I fully model the threads and then pick up the thread root as my contour for the cutter to follow. That usually works, but might require a couple tweaks because the thread mill thread crest is narrower than the part thread root, meaning the pitch diameter will come out a little small if the cutter follows the thread root. I like to make a scrap (or get a real) male plug gauge so I can mike the pitch diameter and get that right and use it to gauge the female thread.

 

[Elemental_Garage]

So to reach a thread height of 0.0722 I'd really need a PDO of 0.0722*2, correct? Which would put the cutter shank into the part.

I never thought about using the root. I just modeled the major diameter as a flat wall cylinder and used the 2d thread path on the wall face.

 

[Elemental_Garage]

We use and love the Ingersoll Rapid Thread family of tooling. If I get what you're saying is that you don't want to drop $200 every time you need to mill a thread, something along those lines will come in handy. Just buy a body or a few if that's what you need and you'll easily be able to find the correct pitch insert for whatever your project is. Bonus that Ingersoll tooling is interchangeable with Iscar and also Tungaloy I believe...you can usually always find what you need in stock from one of those outfits.

Where do you buy your rapid thread stuff from?

 

[Nmbmxer]

If you are making both parts, decrease the pitch until your cutter is happy. I don't think your coolant reservoir will know the difference between 12, 13, or 16tpi on the threads.

 

[VTM]

So to reach a thread height of 0.0722 I'd really need a PDO of 0.0722*2, correct? Which would put the cutter shank into the part.

I never thought about using the root. I just modeled the major diameter as a flat wall cylinder and used the 2d thread path on the wall face.

Per the Machinery's Handbook. The Major Ø of a 2-3/8-12 Is obviously 2-3/8". The Minor Ø is 2.285-2.303. So I would be shooting for the middle of that so 2.294 Minor Ø. So your PDO would be .081 For dead In the middle.

Your cutter should be fine. What is the Minor Ø your cutting your part to?

 

[mr_servo]

McMaster has a thread mill that will do your job for about $65. (edit: your current threadmill has enough reach, actually)

If your only goal is to have two parts fit together and not spend more on tools, you could do a few passes with an axial offset. This will blow out the pitch diameter. I would usually drive a female thread in HSMworks off the nominal major diameter, and due to the sharp point of the cutter, it always has to be moved further out to gage correctly.

If this is a product, it's a different game. You will want to make sure you can make the same thread consistently enough that future parts still fit together, and it would be wise to stay with standard dimensions and tolerances. It's easy enough to measure the male thread with thread wires. The female thread is much harder. In this case, I would suggest making the male thread first, cut the female thread progressively larger until it barely fits, and then make the female thread PD bigger by the amount of clearance you want, which is a lot.

You do not want these threads tight. Aluminum rubbing on aluminum will have a nasty tendency to gall, and it will be worse once one side is buttery soft from welding. Also, welding will shrink the diameter of the thread, possibly by a lot more than you expect.

Anodizing at least the cap and a lubricant or anti seize would help. If the cap doesn't have to be aluminum, there's some pretty awesome plastics out there.

 

[empower]

Thanks for that info. In the context of Fusion, would that height be the same as the pitch diameter offset? View attachment 407792

no, thats not it. read the bottom carefully. is your hole drawn to the minor or major size? same with the boss. if hole is drawn to minor size, you need to add the pitch diameter offset so that the thread is cut to the major size. same with the boss(external thread) - if its modeled to the major size, you need to use the pitch offset so it cuts the threads to correct minor size.
you should be using 2d contour to finish the ID of the hole, and OD of the boss. either add the .01" to the toolpaths, or if using wear comp - put it into the tool offset.

 

[mr_servo]

empower has it. It looks like some are misunderstanding what PDO in the software does, and it's probably because the tool tip isn't very clear. It will put the cutter edge on whatever surface you click on, and then can be adjusted in or out with PDO. It is diameter based, so if it needs to go out .002" radially you would make PDO .004".

Let's say you have a .182" diameter thread mill, put than it for PDO and you can see the center of the tool will be on the selected cylindrical surface.

If you are machining a female thread from a modeled major diameter, the usual case is to have to increase PDO slightly, like maybe a few thou on a small thread and more on a large thread, because of the sharp tip of the typical thread mill vs the little flat on a standard thread, so you need the tip of the threadmill out beyond the nominal diameter. If you click on the minor diameter, you will have to increase PDO to approximately 2X the thread depth, and then some.

Since the Harvey tool comes to a point, you will need to be cutting at least 2.395" at the tip just to have any clearance at all on a nominal 2.375"-12 thread. I think you said you're driving CAM off the 2.375" major diameter, so you're looking at probably around a .040" PDO to get a reasonable amount of wiggle room. Combine that with a minor diameter of around 2.310" and I think you will end up with a thread that will work for you. Your current tooling is fine for that depth. It will also work on the male thread, but there's isn't a lot more room to go. The male thread should have a somewhat smaller flat, meaning the tool needs a little more reach.

 

[Elemental_Garage]

Right now I have both the boss and the hole modeled and cut to the major diameter of 2.375, using pocket or adaptive clearing and then a 2d contour for a finishing pass.

The boss and hole, it seems, I had both set at a PDO of .084, which looked to be about the max I could do before tool interference.

In trying to understand this better I looked up a calc for this and input my specs:



This (above) is for the hole (internal) thread. So this is saying that if my hole is milled to the minor diameter (2.285) I would use a PTO of 0.0911. But, if I had milled the hole to the major diameter my PTO would only be .0101. That would make for some really shallow threads, right?

Now if I look at the external threads:



One thing I don't get here is that it says I have a tooth height of .0138, but that isn't accurate, right? It should be half that since the difference in diameter is split between two teeth. So if I use a PDO of 0.1199 wouldn't that run my tool neck into the part? It looks that way on the simulator. But then the fusion note says it only uses half the PDO value. So it's a little confusing for this newbie!

Thanks all for the help so far.

 

[MaxPrairie]

I use PDO for selecting the minor dia say on a 1/4-20 then set PDO to 0.05 for example. Carmex Tooling also makes indexable threadmills so you have a range of pitches to work with. You also don't need to buy a pack of 10, you can buy just one/two at a time. I think I have a C18 setup from them.

 

[mmurray70]

Iscar and Tungaloy have nice Insert threadmills with a single tooth profile. Great for a wide range of threads, jobshop kinda work.

We have the smaller size in Iscar multimaster. I bought the larger one from Tungaloy because pricing was slightly better. Essentially the same tool. Use them both fairly often. Work great. Get carbide shanks for more reach if you can afford it.

 

[mr_servo]

Internal thread- mill hole to minor diameter, thread mill to major diameter
External thread- mill boss to major diameter, thread mill to minor diameter

So I feel like the problem is coming in because you have a cylinder or cylindrical hole in CAD, and it can't simultaneously be at the major and minor diameter. So either the milling or the threadmilling path will need to be offset. Or both, but one will be offset far more than the other.

I thought you said both are modeled to the nominal 2.375" diameter. But if that's not the setup, then what I write below won't be quite right.

Internal thread, you need to cut the minor diameter significantly smaller than that (closer to 2.3-2.31), and use a small PDO on the threads to get it to gage right, .020 minimum by my calculation for a pointy tool. And that's effectively zero clearance. I think you will want .030 to .040. So to check clearance, 2.375+.04-2.31=.105. This is less than .388-.25=.138, so it won't rub.

External thread, you would mill to a bit below nominal (maybe about .01 below) and use a rather large PDO to get the threads to depth. I would probably model the boss at 2.365 and drive both milling and thread milling off of that. You want the threads to cut to about .126 below your major diameter and would use this for PDO. As you can see, .126 is getting near .138. Here, a PDO of .138 is when things will rub.

The Harvey tool comes to a point. I think this is why there is slight disagreement between my numbers and Saunder's numbers, plus I think you want more clearance than a "2B" thread. I agree that the "tooth height" would seemingly make more sense to be 1/2 of .138, but I want to emphasize this isn't evidence of a math error or clearance problem, just some disagreement over terminology. PDO is a diameter offset and trouble arises when you run out of diameter offset between tooth and shank. If PDO is .100, the tool cuts .05 more radially.

 

[empower]

Right now I have both the boss and the hole modeled and cut to the major diameter of 2.375, using pocket or adaptive clearing and then a 2d contour for a finishing pass.

The boss and hole, it seems, I had both set at a PDO of .084, which looked to be about the max I could do before tool interference.

In trying to understand this better I looked up a calc for this and input my specs:

View attachment 407807

This (above) is for the hole (internal) thread. So this is saying that if my hole is milled to the minor diameter (2.285) I would use a PTO of 0.0911. But, if I had milled the hole to the major diameter my PTO would only be .0101. That would make for some really shallow threads, right?

Now if I look at the external threads:

View attachment 407808

One thing I don't get here is that it says I have a tooth height of .0138, but that isn't accurate, right? It should be half that since the difference in diameter is split between two teeth. So if I use a PDO of 0.1199 wouldn't that run my tool neck into the part? It looks that way on the simulator. But then the fusion note says it only uses half the PDO value. So it's a little confusing for this newbie!

Thanks all for the help so far.

if your hole is modeled to major diameter, how are you roughing and finishing it to the correct minor diameter size?
i wouldnt fuck with the PDO for wear offset, if you need slightly larger, do that in the stock to leave area.