Thread Milling

[Totem]

Hello Ralf,

Your links are interesting, I doesn't know this supplier, are they good quality?

Most of the thread mill bits having a coolant passage (arrosage par le centre) thats why they are as expensive as they are.

Yes. Normal routing bits with coolants passage costs around 90€, the sames without coolant passage 40€, I think it's the same problem with tapping tools.

Like you, at home I tap always by hand or with my drill press... but at school we use thread mill cutters.

I tried to do a threading bit with a chinese endmill, but it doesn't work well: first I tried in wood, OK, then in PVC, but material melted (tos slow feedrate?), and then I broken my tool when trying in aluminium 

++
Lionel

[lloydsp]

Maybe it's possible to do a tool with a modified tap by removing 2 of the 3 flutes ?

---------------------
David,
I have done that, but it's not optimum.  Unless the hole size is very close to the tap size, the helix angle will be to steep, and it will "back cut", changing the thread profile to a badly rounded bottom (major diameter).

The advantage to the nidexable lathe bar is that inserts are available with a variety of rake angles and helix angles.  It makes a nice thread.

Lloyd

[pixelmaker]

hello,

@ lionel

I doesn't know this supplier, are they good quality?

yes, It is a tool dealer for metalworking tools, good quality but normaly not the cheapest.
like Leitz tools for woodworking and crown norge for the best PMMA cutting tools. They send out from stock in france, fast and without tax for norway. But be carefull, this cutters are very sharp.

With everything I've read in last days about thread milling tools, it is actually more useful to work with cutters like at the attached image? The circular motion is what the plugin generates.

In the german section on the screenshot there is in front a additional value "p" . This must be the thread pitch.
Maybe someone can tell me whether it is as I understand it.

With the first cutter I can cut a metrical thread M (60°) inside from 6mm ( diameter 5. up to 11mm (pitch 1.5) and outside I can cut from 3mm (pitch 0.5) to 11mm. Pitch = depht increment.
Is this right?¿

the catalogue is here - 06 Circular and Thread Milling

ralf

[Totem]

Hallo Ralf,

In the german section on the screenshot there is in front a additional value "p" . This must be the thread pitch.
Maybe someone can tell me whether it is as I understand it.

With the first cutter I can cut a metrical thread M (60°) inside from 6mm ( diameter 5.8 ) up to 11mm (pitch 1.5) and outside I can cut from 3mm (pitch 0.5) to 11mm. Pitch = depht increment.
Is this right?

For internal threadings I understand like you, but normally those mills are NOT made to mill external threadings.
It's simply because their angle is not really 60°, but about 47/49, to compensate movement angle: so, to do a 60° threading, you must always use those tool at helix angle there are made for.

You can't do smaller or bigger pitch as normal M, for example if you try to do a 10mm thread with only 0.5mm pitch instead of 1.5, the helix angle will be smaller, and so, the angle of the filet will be less as 60° to.

Hope you understand, if no, I can do a draft of the problem with SW for you.

++
Lionel

[nzinoz]

hello,


With everything I've read in last days about thread milling tools, it is actually more useful to work with cutters like at the attached image? The circular motion is what the plugin generates.

In the german section on the screenshot there is in front a additional value "p" . This must be the thread pitch.
Maybe someone can tell me whether it is as I understand it.

With the first cutter I can cut a metrical thread M (60°) inside from 6mm ( diameter 5. up to 11mm (pitch 1.5) and outside I can cut from 3mm (pitch 0.5) to 11mm. Pitch = depht increment.
Is this right?¿

the catalogue is here - 06 Circular and Thread Milling

ralf

Hi Ralf from what I understand you can cut .5 to 1.5 thread pitch. the V is not sharp enough to cut finer and not large enough to cut bigger pitch. You should be able to cut any Diameter with a 1.5 pitch. You could cut a 20mm x 1.5 pitch.
The thread form is only the pitch by the depth of cut making vvvvvv or VVVVVVV .  

[pixelmaker]

hello Lionel,

normaly there are different cutters for nut and bolt threads.
The cutter in  Andy´s article has the helix specially for only one size of thread. The spacing of the threads is fixed.
The cutter in my post has no complete helix. The distance of the threads can be determined by depth increment.
If I understand this correct, I can cut with this two cutters all inside threads ISO M from 6mm to  16mm.
The price of the two cutter together is lower then the price of one of the cutters like Andy show it.
If I buy this thread mill cutters I do this only for cambam tests.
For daily use I have a Fein ASg 648 thread cutter for the nuts and a REMS thread cutter system for the bolts.

What is the advantage/disadvantage of the helix thread mill cutter like on the picture of Andy against this one on my picture?

@ nick, I think the blades are tilted some degrees and this gives the restriction for the pitch.

ralf

[lloydsp]

What is the advantage/disadvantage of the helix thread mill cutter like on the picture of Andy against this one on my picture?


------
Ralph, a "full profile" threading mill can mill a thread as long as its cutting length in one revolution around the cavity.  "single-point" tools require that the tool tip trace the entire thread path from (normally) bottom to top of the cavity.

The disadvantage of a full profile tool is that it cuts only a very narrow range of helix angles and depths, and can cut only one pitch.  A single-point tool can cut a fairly wide range of threads.

LLoyd

[Totem]

Hello Ralf,

I'll made a drawing for you this afternoon, so you will understand why you can't do external threading or finest pithch as normal pitch. (I can't explain it in english)

++
Lionel

[pixelmaker]

Lionel,

you must not make a drawing.

I found now a short video where they cut a thread inside aluminium without drilling a hole. In a short moment you can see the cutter and it looks like this one on my foto, only .

Lloyd, thank you. I understand now. Cutting with a single point tool brings the tolerances of the machining into the threads. The forces on the the blades are higher. This tools are only usefull for larger diameter threads.

ralf

[lloydsp]

Oh, Ralf!  That's very nice.  I had not seen single-point tooling that was also end-cutting!

Lloyd

[10bulls]

I'll made a drawing for you this afternoon, so you will understand why you can't do external threading or finest pithch as normal pitch. (I can't explain it in english)

Thank you for your explanations Lionel.  I think your English explanation was very good... it is just a bit of a tricky concept to convey.  I'm struggling to think of a better way to say it without pictures too.  

I originally wanted to get a single tip cutter. As Lloyd says, you do have a lot more variety on the range of pitch threads you can cut.  The threads will take longer to cut and the cutter will wear quicker for single flutes, but for experimentation this wouldn't have been so bad.
However, I went for a multi-flute mainly because it was a lot cheaper.  Being faster to cut threads they are more common 'stock' items.  I didn't spend too long shopping around, but even though the multi-tooth was still expensive, a single flute would have been a custom grind and about twice the price.
I've also mostly standardised on M6 for my medium sized widgets and gizmos I make, so the M6 multi-tooth cutter should pay for itself with time saved pretty quick.

[Totem]

Hello.

you must not make a drawing.

It's too late  

When I read your message, I already made my drawing.

I doesn't drawed an internal threading, because it's more difficult to understand the problem in this configuration.
To simplify, I will made a simple "filet" (not sure it's the right word, what I think is filet en français / gewinde auf deutsch) at the side of a box, as on this picture:



But with differents angles.

First sample: toolpath angle is around 7°

Here I set the cutter as transparent.

You can see that the upper and lower face aren't generated at the same (red/green) depth.



If I cut the view, you can see that filet angle is NOT the same as tool angle, due to toolpath angle.



But the difference is pretty low...

Second sample: I do the same experiment with 28° angle (OK, in real a thread is never more as 15°, but so you see better the difference between the two angles)



Now, the shapes of the filet is not exactly the same!



I hope that you understood the influence of the toolpath angle on the filet shape...

And at this picture (from David), you can easly see that path angle is NOT the same for internal or external diameter!
It's why internal milling tools should NOT be used for external diameters..



++
Lionel

[pixelmaker]

Thank you Lionel,

while you paint your picture I grind my first thread mill cutter. 
I grind it from a broken 6mm 1 flute solid carbide cutter. The tip is the original cutters blade, for this I have a 6mm pitch circle. The tip has ~60°, at my grinding machine there is one scale I have to repair for correct grinding.
Tomorrow I will try how it works, in PMMA. I will post the results, I hope tomorrow.

Time is running. Till sunday evening I have to finish my first work in 3d printing. Today I get the first of the printed figurine, I make the infiltration with PMMA. Now I have to grind it, then coat it with silver, put a printed sign between their hands and then cast it into a pmma block with screenprinting inside. The 3d print comes with a delay of 3 days and it is just as much work as it sounds. It has nothing to do with cambam, but I like it. The sculpting I do with Zbrush, also my first work with this software.

[nzinoz]

Hi Lionel I understand what you mean but the cutter is not a 60deg disc, it is 4 individual teeth each with the back face relived see magnified photo

[Totem]

Hello Ralf,

I've tried too to do a thread cutter with an old endmill, but mine doesn't work (but I've no grinding machine, I tried with a simple grinding reel, it wasn't really sharp  )

Hop yours will made a good result...

Your 3d printing is really pretty, what are you using for a 3d printer? DIY or not  ?

Hello Nick,

I understand what you think, but when the spindle rotate, the sharpened ridge turn and do like my disc.

Your picture is good quality, what do you use for a camera?

++
Lionel