Thread milling: Single point thread mill vs. inserted threading bar

[greenbuggy]

I've finally got my Lagun CNC mill up and running, and I want to try thread milling with it.

I've checked out some single pitch thread mills, and holy crap are they expensive. Seems to be that the ones that will do reasonably low thread counts are $150+ in carbide.

I don't expect to do too many real oddball threads, but I have one project that is going to require an 8 TPI outside thread, and I don't want to spend $150 to do it.

So I was wondering, since speed isn't terribly important on this one off job, could I slow my feed down and instead of using a single point thread mill, use an inserted threading bar like this one: 12 1 2 Mini Indexable Threading Tool Holder Inserts Set | eBay instead?

What kind of range of TPI does an indexible threading tool have as compared to a single pitch carbide? For comparison the $150 single pitch one I was looking at could handle 6-32 TPI. Link: 1" 6 32 TPI Single Pitch Thread Mill Brand New TiAlN Coated | eBay

I see it says it'll do 16-48 TPI but are there other inserts that will fit to do larger sizes?

I have future uses for thread milling but I'd like to get into it without spending a ton of money if possible, and if possible leave myself open to the maximum range of thread options without buying more tooling

 

[i_r_machinist]

I run lathe threading bars on my cnc mills, but this isn't a production shop. Works fine.
i_r_

 

[CougarMountain]

A single point thread mill will work fine, but slower as you said. Also you may have a bit more of a burr on the crest to polish off, whereas a multi-tooth mill would leave a clean thread form. I favor the endmill style threadmill with a slow spiral, as they do not seem to hammer as much on thin parts as an insert multi-tooth style. Yes, they are expensive, but they really seem to last, and I was doing mostly titanium. Ymmv

 

[upnorth5axis]

I have used a similar indexable tool for thread milling and it works fine. You may have a problem finding inserts that will be big enough for an 8 pitch and remember this won't be the fastest way to do them. I have also used the single pitch threadmills and they work better than the indexable and you can feed faster. I personally don't like the corn-cobb multi-pitch models for small sizes. they tend to break to easily.

 

[NTM]

Lakeshore Carbide has (finally) added single profile thread mills to their lineup. Like their endmills, they're high performance at a good price. :

LakeShore Carbide.com Carbide End Mills-Carbide Thread Mills - SINGLE PROFILE ALTiN COATED THREADMILLS

8 TPI is a big damn thread, but looking at the major diameter and minor diameter it looks to me like their largest (which is shown as a 10 tpi to 32 tpi) should be able to cut an 8 TPI. You may need to run a finish pass with a Z tweak to hit your pitch diameter but the minor diameter is there. $90 for such a big thread mill is a good deal.


Nathan

 

[Nami]

I've bought both the 6-32 and 5/8-18 threadmills (full form) from Lakeshore and they are the only way to go as far as I'm concerned. The 6/32 was for a very shallow hole (0.125") in 6061, and I tried cut taps / form taps / rigid tap/ compression holder trying to dial it in. Finally got the threadmill from Lakeshore after talking to their guy Carl ( a real standup guy). Told him I broke one due to my fault, and he still sent me a free one, then proceeded to hold my hand until I got it dialed in. Went on to tap 400 holes without a hitch, and they look better than any of the other methods.

Because they have multiple teeth and are a "topping" cutter, the threads really look fantastic, go within 0.005" from the bottom of the hole, and were actually faster per hole than any of the other methods, at least on my machine.

Don't cheap out on this; call them and tell them what you are trying to accomplish, and take their advice on speeds / feeds /etc. You won't be sorry.

 

[67Cuda]

Take a 2 or 4 flute tap of the same pitch, grind off all but side of the flutes and use that. At the very least if you want to use an off the shelf system, you can practice thread milling.

Tom

 

[DDB]

Take a 2 or 4 flute tap of the same pitch, grind off all but side of the flutes and use that. At the very least if you want to use an off the shelf system, you can practice thread milling.

Tom

Really? I never thought of this or heard of this before. Have you tried it? I am interested now. Could be a damaged tap that just might be worth trying but I wondered if you have really done this.

 

[craigS]

I have done this with a tap, it works out ok but the tap doesn't last too long. You need to grind off all but one tooth and add some relief clearance to the back side of that single tooth. I managed to cut some 1.25" x 12 internal thread .6" deep on a couple of pieces of steel DOM tubing then make some matching external threaded end plugs from aluminum. Would be nice to afford a real thread milling cutter, but I couldn't justify it for just two non critical parts. The first attempted looked perfect except for a G-Code screwing up, I cut a really nice left hand thread, DOH!

Craig

Craig

Really? I never thought of this or heard of this before. Have you tried it? I am interested now. Could be a damaged tap that just might be worth trying but I wondered if you have really done this.

 

[Captdave]

8 TPI is a big damn thread, but looking at the major diameter and minor diameter it looks to me like their largest (which is shown as a 10 tpi to 32 tpi) should be able to cut an 8 TPI. You may need to run a finish pass with a Z tweak to hit your pitch diameter but the minor diameter is there. $90 for such a big thread mill is a good deal.

have several of their thread mills and have had really good luck with them and have good tool life.

Did a batch of 3/4-10 x1" internal threads with a multi flute tool and it took 3-4 passes with a spring pass to get it dead nuts. IIRC I think we ran it at 30-40 IPM. There was no speed/feed posted so I wondering if on a 10 TPI thread with a single flute if you could do that thread in 1 pass at maybe 30 IPM considering there would be a lot less tool pressure to consider?

 

[Red James]

I made my first threading tool holder to use TPG inserts . . .3/8 I.C. if I recall. Worked great! Once I determined the effective diameter of the homemade tool I could get very close to any thread I needed. True, this is not the fastest method, but if you only need one or two threads of a particular pitch, it sure beat buying thread mills.

 

[SIM]

I made my first threading tool holder to use TPG inserts . . .3/8 I.C. if I recall. Worked great! Once I determined the effective diameter of the homemade tool I could get very close to any thread I needed. True, this is not the fastest method, but if you only need one or two threads of a particular pitch, it sure beat buying thread mills.

Been there done that.

I did my first helical threadmill with a HSS tool it in a steel boring bar.
Worked fine and cheap.

Second was a HSS wood drift style key cutter with 60 deg angle as I was too cheap(scared) to buy a real carbide cutter. Worked very well as multiple teeth allow for a fast feed rate. Compared to single point HSS. I still keep one of these in my draw for those odd thread pitch jobs it just don't pay to buy a carbide threadmill. Just cannot get to the very bottom, nor go very deep.

Another good option to get deep is an indexable lathe threading bar.
It's a slow process, but can spin pretty fast so feed isn't too bad, but you can thread pretty darn deep going this way.

I then needed to do an OD 1"-20 in alum. Still to cheap and weary to buy a carbide tool I opted to modify a tap. Cut two of the three flutes off and tried with poor results. I found the helix was rubbing and needed to remove more of the trailing edge. Worked good after that... Although it was only alum.

That gave me the comfort to order a carbide threadmill the next time job came up and found that was the ultimate in speed accuracy and finish but at significant upfront cost.

But as long as you don't Ooops they last and last in the most challenging materials.

 

[spock]

I make these and they do pretty well. Simple as it gets.

 

[bevinp]

I make these and they do pretty well. Simple as it gets.

Are they carbide or HSS? What stops the insert from turning? How much to buy from you?
Bevin

 

[Brian]

Spock,

Your method there won't work, your thread form is incorrect because the 60º point on your insert is not at 90º to the cut. If that same insert was used using just one corner and it was on centerline of the shaft's axis, it would work. I haven't done the math, but I bet your thread angle is closer to 65º the way you are doing it.... cut a groove in a block of material and put it on the comparator, that will tell you what it is.

 

[Oldwrench]

...your thread form is incorrect because the 60º point on your insert is not at 90º to the cut...

Keerecto. Your edge has a huge negative rake which flattens the vee profile. Relocate the screw and backstop so your edge is radial like a boring tool. The minimum bore will be substantially larger but the thread form will be right.

 

[SIM]

Are they carbide or HSS? What stops the insert from turning? How much to buy from you?
Bevin

Really?
It's a rod with a tapped hole in the end. Direction of cut tightens the screw further.


And to the form being off...yes it would, not going to pass lots of inspections. But for many jobs I think it would work fine, especially if only roughing a thread to be chased with a tap or light duty mechanical joints. Long as customer knows what is being offered.

 

[Red James]

Even better than my original . . . but I did not have laydown inserts available. I like this one!

 

[spock]

My pic might not show it but there is a triangle pocket milled in the bottom of the rod, that fits the insert pretty well. That takes the force, and the screw keeps it from falling out.

The inserts I have on hand are not 30 deg per side, they are in fact 32. They leave a 64 degree (if you cut a block and check on comparator, as mentioned above) unless you alter the factory angle on the insert.

 

[Bruce Griffing]

Clearance is important. I would not use a thread mill that is designed to cover a certain pitch range for a thread outside that range. So if you do buy a single point thread mill, make sure it covers your desired pitch.