[DLawrence]

I am approaching thread milling for the first time...I need a whole lot of 1/2-13 holes threaded 1 inch deep in 12L14

Wondering what the pros and cons of the single lip miller such as Tormach sells vs full depth cutter like Maritool sells.

Also considering grinding down a "trial thread miller" from a carbon steel tap , a 3/8-16 or 7/16 and leaving just one thread like the pictures of the

carbide single lip millers ,........ just to see the process work one time ....at somewhat reduced thread depth....... and verify the feeds/speeds before trying an expensive carbide cutter.

Any thoughts?

Dave Lawrence

[SCzEngrgGroup]

Are you asking about a single-point, vs multi-point thread-mill? If so, the differences are: Multi-point is faster, a lot more expensive, and can cut only a single thread pitch. Single-point is slower, cheaper, and each tool can cut a wide range of pitches. In terms of thread quality, there is no major difference, when properly used.

Regards,
Ray L.

[cbyrd]

John Saunders at NYC CNC did a video on Thread Milling..

https://www.youtube.com/watch?v=uHIG49ZZYVY

Might be helpful.

Chris

[TurboStep]

The price difference is not THAT huge. Yes the single profile thread mills are a little more flexible but there are limits. It's not like you can cover all your threading needs with just one tool. For common threads I use the full length type but I have a couple of single form thread mills to cover the less often used ranges. For me it's a trade-off between cost and convenience. For some it would be initial cost vs time saved. A full length thread mill is a lot faster so your statement:

I need a whole lot of 1/2-13 holes threaded 1 inch deep in 12L14

implies to me that would benefit from using a full length type, depending on how many a "whole lot" really equates to. Divide the cost of the thread mill (or the difference in cost if you prefer) by the number of threads. Then determine how much your time is worth!
I would also check out the variable flute thread mills from lakeshorecarbide. I haven't tried this type myself but their variable flute end mills are great.
Step

Edit: almost forgot, the full length types create threads with the correct thread form and will automatically give you the correct thread diameter. Single form thread mills are ground almost to a point and if the cutting diameter is used for the calculations without compensation you are likely to obtain a tight or "interference fit"!

[mountaindew]

. Single form thread mills are ground almost to a point and if the cutting diameter is used for the calculations without compensation you are likely to obtain a tight or "interference fit"!

I like that term!

What is the term when you use the same single point tool for both id. and od threading? I found with a little experimenting and you can get some crazy close fit threads.



Should have known when I seen link to recent nycnc video above, was checking my email and some of my single point cutters I ordered last week are on back order and will not arrive with my backup Hamier probe tips , oh well these were backups also.

[Steve Seebold]

Are you asking about a single-point, vs multi-point thread-mill? If so, the differences are: Multi-point is faster, a lot more expensive, and can cut only a single thread pitch. Single-point is slower, cheaper, and each tool can cut a wide range of pitches. In terms of thread quality, there is no major difference, when properly used.

Regards,
Ray L.

AND with a multi point thread mill if you need to recut your thread, you're screwed because there's no way to pick up the thread to recut it. With a single element tool, it's easy.

[CadRhino]

Another thing to check is the depth of threading you need to do. Often single points can thread deeper.

AND with a multi point thread mill if you need to recut your thread, you're screwed because there's no way to pick up the thread to recut it. With a single element tool, it's easy.

[greggv]

1/2 13 in 12L? Why not just tap it? Would be faster

[TurboStep]

AND with a multi point thread mill if you need to recut your thread, you're screwed because there's no way to pick up the thread to recut it....

are you really sure about that???
Step

[TurboStep]

For anyone who's wondering, a multi-point thread mill will pick up the thread in exactly the same manner as a single point.
A multi-form thread mill for about $105 isn't that much more expensive than a single point thread mill capable of cutting the same thread. Also, don't forget that a single point thread mill has only one row of teeth. A 1/2-13 multi-form thread mill with a cutting length of 1" will have 13 rows of teeth to do the same work, will therefore last a lot longer, so will actually work out significantly cheaper in a production environment, and that's not even considering the time savings.
Step

[Hirudin]

I'd recommend starting with a single-point mill. It'll make your threaded holes and give you some experience with thread milling. After a while I bet you'll want to go with multi-point mills for the time savings. At that point, you'll have a nice 60° back-chamfer tool for later.

Feel lucky that you're doing such large holes. My first attempt with thread milling was some 6-32 holes and I used a multi-point thread mill. This was with a TAIG mill. The first hole seemed to go OK. The second snapped the tool almost instantly.

[tbev]

I use the singles from Tormach, they are great. Aluminum, titanium, delrin, same bit, lots of holes, it's super nice to be able to play with the major/minor Dias, pitch etc ... I couldn't be happier...I don't think anyways.

Sent from my SM-G900V using Tapatalk

[DLawrence]

Standard Feedrate calculator on lakeshore carbide site says .0025 -.0035 (inches/tooth) feed in low alloy steel for 1/2-13

I just got a single form FOUR flute 3/8 tool cutting dia

I think some single form tools may have 6 teeth ...they would feed in faster wouldnt they ? a full depth cutter with 13 rows of 4 teeth

't it (52 teeth times .0025 ?) wouldn't it need to feed in slower? Whats the principal behind this (inches/tooth) stuff ?

How can I use the inches/tooth to determine feed in PP conversational ? or in handwritten Gcode ?

Thanks
Dave Lawrence

[Philbobb]

Diametral teeth, not vertical teeth. Treat it like a 4 flute end mill. 0.0025/tooth x 4 flutes = .010"/revolution.

[SCzEngrgGroup]

Unless PP allows you to correct for path radius, using a feed/speed calculator will give you the wrong feedrate. For a threadmill, the effective feedrate at the cutting teeth is much higher than the linear feedrate in the g-code F-word, due to the small path radius. Good F/S tools (like HSMAdvisor) will calculate the correct values, based on the tool and thread diameters, chipload, etc.

Regards,
Ray L.

[DareBee]

Standard Feedrate calculator on lakeshore carbide site says .0025 -.0035 (inches/tooth) feed in low alloy steel for 1/2-13

I just got a single form FOUR flute 3/8 tool cutting dia

I think some single form tools may have 6 teeth ...they would feed in faster wouldnt they ? a full depth cutter with 13 rows of 4 teeth

't it (52 teeth times .0025 ?) wouldn't it need to feed in slower? Whats the principal behind this (inches/tooth) stuff ?

How can I use the inches/tooth to determine feed in PP conversational ? or in handwritten Gcode ?

Thanks
Dave Lawrence

You don't need to handcode. Download a free thread coder from a threadmill manufacturer and cut&paste the code.

A threadmill will cut a 1 inch deep thread in 2 passes (a few seconds) vs 26 - 39 passes for a single (min+/hole)