CNC Thread Milling M2

[fumopuc]

Hi everybody, another interesting issue for the CNC mill.
The other day I have made a round hole pattern for M1,6 mm holes and this followed by the usual thread cutting by hand.
After some threads getting a tired wrist and the question in my mind why do you not do it with the mill ?
Theoretically an easy thing.<a href="https://www.youtube.com/watch?v=0v2VKG8lcNo" target="_blank">http://www.youtube.com/watch?v=0v2VKG8lcNo</a>
For a M2 test milling I have bought a cheap cutter here in Germany.
First test was done in wood, followed by five M2 threads into an aluminium plate.
The movement of the table is nearly not visible.
<a href="https://www.youtube.com/watch?v=TT-xrplIJrQ" target="_blank">http://www.youtube.com/watch?v=TT-xrplIJrQ</a>


I would say a good experience for future projects.

[Jasonb]

That is not something I have tried yet but may have to add a cutter onto my next order to try it out.

[Dave Otto]

Nice work Achim, that is one tiny little cutter.
Thread milling can be quite useful, attached are some photos of the body castings for the 4 post oilers I made for my Pacific engine. All the external threads were milled.
I made a set of printed soft jaws that orientated each boss. After each machine cycle the castings were shifted to the right and the right most one was complete. The holes were also drilled in this step.
Also great for doing tapered pipe threads.

Dave

[Hugh Currin]

fumopuc: Nice. Likely a lot easier to dig a broken milling tool out than a broken tap.

Dave: Formed soft jaws. Another reason to obtain a 3D printer.

Thanks.

[Dave Otto]

fumopuc: Nice. Likely a lot easier to dig a broken milling tool out than a broken tap.

Dave: Formed soft jaws. Another reason to obtain a 3D printer.

Thanks.

Especially if you have the 3d CAD for the part you are machining.

Dave

[Muzzer]

These thread mills can be furiously expensive. However, I bought some thread mills from yuzemachinery.com (Rickie) for between $5.90 (M3) and $10.10 (M8) plus carriage. Having said that, my first internal thread milling job was an M16 thread, for which I actually used a Simturn boring bar with an internal threading insert as a single point cutter. Solid carbide single point cutters for M16 would have been about $28 each, with little likelihood of ever being reused. Besides, I already had a boring bar with appropriate threading inserts.

When creating the toolpaths in Fusion, you need to understand what is meant by "pitch diameter offset", as you need to enter a value. In simple terms, it's the amount of infeed you need in order to give the correct thread depth ie the radial difference between the OD and the bottom of the trough. That will be a bigger number if you have a pointy ("agnostic") tooth profile.

[fumopuc]

I have done some experiments with this pitch diameter offset already.
Decreased by 0,1 mm and it was impossible to get the bolt Into the thread.
Decreased by 0,05 mm and the bolt can grab the first part of the thread but impossible to go further.
So very sensitive and nice for any adjustment in both ways.

[john mills]

interesting ahead milling in these sizes  i have only used industrial machines even a smaller light machine and lathes with live tooling
which do those size threads eagerly using taps  the old machines with floating tap holders could be interesting too the modern machines with rigid tapping do it easily so would never think of thead milling .
John 

[Jasonb]

The other advantage is that you can cut non standard threads that a suitable tap would be hard to come by for example if you wanted to screw a model engine cylinder into a crankcase M25 x 1 would not be a problem. So a few mills in the common metric constant thread pitches would allow you to cut a vast range of threads.

And thinking of Craig's radial you could get all the threads starting at the same point so all the cylinders should line up when screwed in

[kvom]

That's single point thread milling, where the tool can cut a variety of threads limited by the thread depth and the ramp angle ground into the teeth.  With a blind hole like this example you want to spiral upward as the swarf falls below.  With the through house ramp down as the swarf falls out.  The same tool can cut left or right hand threads, internal or external.

Something to consider is SFM in defining feedrate. SFM using only tool diameter and RPM fails because tool path isn't straight.  This is true of any arc toolpath, but can be important with small tools. 

Internal Feed = [(Major Thread Dia - Cutter Dia) / Major Thread Dia] x Linear Feed

External Feed = [(Major Thread Dia + Cutter Dia) / Major Thread Dia] x Linear Feed

[Muzzer]

Worth noting that a RH thread being climb milled will start at the bottom and end up at the top.

[fumopuc]

That's single point thread milling, where the tool can cut a variety of threads limited by the thread depth and the ramp angle ground into the teeth.  With a blind hole like this example you want to spiral upward as the swarf falls below.  With the through house ramp down as the swarf falls out.  The same tool can cut left or right hand threads, internal or external.

Something to consider is SFM in defining feedrate. SFM using only tool diameter and RPM fails because tool path isn't straight.  This is true of any arc toolpath, but can be important with small tools. 

Internal Feed = [(Major Thread Dia - Cutter Dia) / Major Thread Dia] x Linear Feed

External Feed = [(Major Thread Dia + Cutter Dia) / Major Thread Dia] x Linear Feed

Kirk, some help needed
Does SFM means Surface Feet per Minute ?

[Jasonb]

Yes, it would be the imperial of Vc in feet per min rather than m/min

[dieselpilot]

Surface speed is not the issue here. The formula presented compensates feed rate relative to cutter and feature diameter to maintain desired chip load. This is a concern for all tools, no matter the size, but for thread milling it's quite pronounced and they are often fragile.

[Muzzer]

Is that really a concern? This putative feedrate "error" will be of the order of the thread depth divided by the radius which is typically about 20% for metric coarse threads. The feed per tooth values recommended by the manufacturers are usually defined as a fairly wide range and I would expect most of us to err towards the safe end of that range, given the cost and fragility of these things. Feedrates recommendations, rather like surface speeds, are fairly directional, not a precise requirement.