thread milling?

Here's the place for discussion related to CAM/CNC and the development of the Path module.
Forum rules
Be nice to others! Respect the FreeCAD code of conduct!
Post Reply
User avatar
JoshM
Posts: 456
Joined: Thu Oct 05, 2017 5:34 pm
Location: New Hampshire

Re: thread milling?

Post by JoshM »

The other day I noticed that there are tools for internal threading, for external threading, and for both. I have no idea what the difference is and why one would be only usable for internal or external, but not both--anyone know any more about this?
-Josh
Bendall
Posts: 41
Joined: Sat Oct 10, 2020 2:25 pm

Re: thread milling?

Post by Bendall »

JoshM wrote: Mon Dec 21, 2020 10:37 pm The other day I noticed that there are tools for internal threading, for external threading, and for both. I have no idea what the difference is and why one would be only usable for internal or external, but not both--anyone know any more about this?
-Josh
That's interesting, as far as I am aware they should be usable for both. The deciding factor for internal is if it will fit in the hole. And they they are only good for a certain threads pitch otherwise you will rub on the shaft. But external ones can be as big as they want to be because there isn't a clearance problem.
User avatar
JoshM
Posts: 456
Joined: Thu Oct 05, 2017 5:34 pm
Location: New Hampshire

Re: thread milling?

Post by JoshM »

I looked at MSC Direct and sorted by external only (only 28 options compared to 138 for internal) and I can't see an obvious difference with this 16 TPI, External Single Profile Thread Mill.

https://www.mscdirect.com/product/details/60374675

Image

BTW, I know what you mean about external being less constrained, but that really depends on the surrounding 3d shape, because you need clearance equal to the tool tip diameter around your threads.
mlampert
Veteran
Posts: 1772
Joined: Fri Sep 16, 2016 9:28 pm

Re: thread milling?

Post by mlampert »

IIRC the kerf on the internal thread is smaller, meaning the "thread" is pointier - if that makes any sense. But it would be great to get clarification from the manufacturer if that is indeed the difference.
GeneFC
Veteran
Posts: 5373
Joined: Sat Mar 19, 2016 3:36 pm
Location: Punta Gorda, FL

Re: thread milling?

Post by GeneFC »

mlampert wrote: Tue Dec 22, 2020 12:41 am IIRC the kerf on the internal thread is smaller, meaning the "thread" is pointier - if that makes any sense. But it would be great to get clarification from the manufacturer if that is indeed the difference.
Yes, there is a profile difference between internal and external threads. This can be seen in various handbooks. Here are a couple of examples.

Capture-UNC.PNG
Capture-UNC.PNG (17.86 KiB) Viewed 3692 times
Capture-metric.PNG
Capture-metric.PNG (16.83 KiB) Viewed 3692 times

Every thread standard has its own specs with respect to shape.

For most hobby machinists, like me, this is of minimal importance. For precision industrial work the profile is often very important.

Gene
bmsaus4ax
Posts: 255
Joined: Sat Nov 14, 2020 9:16 pm
Location: Bargara, Queensland, Australia UTC+10

Re: thread milling?

Post by bmsaus4ax »

JoshM wrote: Mon Dec 21, 2020 10:37 pm The other day I noticed that there are tools for internal threading, for external threading, and for both. I have no idea what the difference is and why one would be only usable for internal or external, but not both--anyone know any more about this?
-Josh
posted late, after others replied. (I'm slow)
It is all to do with how they are mounted.
We traditionally run lathes with spindle rotation toward us from top view and tools mounted face up, this gives us our right to left paths. The helix angle for the internal threading tool as a result angles from top left down to bottom right, " \" looking down from the top( direction the material is approaching from). If you take an internal tool and use on the outside the helix for the tool is now top right to bottom left " / " the clearance angles are now opposite for the thread helix " \ ". A tool for both will have both edges ground for clearance on both sides " \|/ " and be weaker as a result , which is not the problem it used to be before carbide tools.
The internal tip can be used if it is mounted so as to run on the back of the stock with the spindle running in reverse, the material is approaching the top of the tip from the same relative direction. Most manual centre lathes don't have the cross slide travel to do this.
Thread milling solution is that right hand internal threads are cut from the bottom up counter clockwise G03 , and right hand external threads are cut from the top down clockwise G02. Haven't seen a left hand thread mill.
Photo attached as screen shot Credit to Carmex Precision Tools Ltd document at https://www.samtectools.com/pdf/threadi ... urning.pdf
If you want information overload on threading there's this ridiculously long link but that is what copied from SANDVIK Coromant https://tibp.blob.core.windows.net/coro ... 20-031.pdf
Attachments
Screenshot from 2020-12-22 09-21-48.png
Screenshot from 2020-12-22 09-21-48.png (371.17 KiB) Viewed 3686 times
GeneFC
Veteran
Posts: 5373
Joined: Sat Mar 19, 2016 3:36 pm
Location: Punta Gorda, FL

Re: thread milling?

Post by GeneFC »

While this is all correct for ordinary lathe turning of threads, it really does not apply to thread milling. A snapshot from the Sandvik document referenced shows that the threadmill shape is not adjusted for left-handed or right-handed threads.

Capture.PNG
Capture.PNG (11.58 KiB) Viewed 3637 times

I believe the primary reason for differences in inside and outside threadmills is the profile, not helix tilt.

Gene
User avatar
JoshM
Posts: 456
Joined: Thu Oct 05, 2017 5:34 pm
Location: New Hampshire

Re: thread milling?

Post by JoshM »

Just wanted to say thanks for the discussion. It's always nice to learn, and to benefit from others experience. I have no experience with turning, and limited experience with milling, so the finer points are sometimes lost on me.

Just for giggles, does anyone know why the single-profile style cutters like the one I linked above are called "Scientific" cutting tools? Do they require that the user is a scientists, or????
tigr180
Posts: 25
Joined: Thu Oct 08, 2020 3:37 pm
Location: Taiwan

Re: thread milling?

Post by tigr180 »

Good infos came recently. Thank you all for it.

I checked with one manufacturer about the inside outside threading cutter. They told me I can use the inside tool also for outside thread it obviously has to do with the relief angle tools for outside do not have to be as pointy as inside tools. ( not as pointy means stronger )

I milled left hand and right hand threads. They can be cut with the same cutter no problem. Just the helix must be left or right hand. Outside right hand thread: Milling start at the top and moves -z during cut. Left hand thread, the cutter first move down next to the part and then spirals upwards. Example was bottom bracket adapters for BSA thread. (6xxx Al T6)

The side relief that bmsaus described for the lathe tool must apply in some form for a milling tool too. I guess for my example it did not matter anyway, because BSA threads have 24 tpi, a little over 1mm. Together with the larger diameter, the helix angle of the side is very low, even if it rubs the rubbing will not ruin it I guess. I do not have any metrology tools ( or skills ) to check the quality of the parts. My gauge is a cut out from a bicycle frame as nut :-).

Unfortunately the parts have outside thread, so I was not using FreeCad ( not yet ).
bowcoastie
Posts: 17
Joined: Tue Sep 10, 2019 2:04 am

Re: thread milling?

Post by bowcoastie »

Good morning everyone,
I downloaded Cox's example and Sliptronic's tool definition and it worked well as can be seen below:
Threadmill1.png
Threadmill1.png (286.59 KiB) Viewed 3460 times
I have also updated to the latest development version but I don't have the button below in the available operations:
Threadmill2.png
Threadmill2.png (4.74 KiB) Viewed 3460 times
Is there something else I need to download to get the threadmilling operation in my version of FreeCad?

Thank you to all who have made this feature available; I am truly astounded by your brilliance and generosity!

My version is as follows:
OS: Windows 10 (10.0)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.23756 (Git)
Build type: Release
Branch: master
Hash: 9c6e9184930a52b165a0b7274e3a45d1006bfe67
Python version: 3.8.6
Qt version: 5.12.5
Coin version: 4.0.0
OCC version: 7.4.0
Locale: English/United States (en_US)
Post Reply