thread milling?

Here's the place for discussion related to CAM/CNC and the development of the Path module.
User avatar
JoshM
Posts: 456
Joined: Thu Oct 05, 2017 5:34 pm
Location: New Hampshire

thread milling?

Post by JoshM »

Been a while since I've looked much at PathWB, and what a lot of nice improvements!

I searched and didn't see anything yet in place for cutting threads using a thread-mill, and figured I'd ask if anyone has experience with setting it up in PathWB. Is it as simple as using the Helix operation and setting up the Helix operation exit? If so, is there a long-term way to integrate it so that the G-Code can be generated from actual threads in a model?

Image

Best,
Josh
chrisb
Posts: 37776
Joined: Tue Mar 17, 2015 9:14 am

Re: thread milling?

Post by chrisb »

Before doing this we would need a FreeCAD thread. The hole feature from PartDesign could well serve for that.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
GeneFC
Posts: 2817
Joined: Sat Mar 19, 2016 3:36 pm
Location: Punta Gorda, FL

Re: thread milling?

Post by GeneFC »

JoshM wrote: Wed Aug 19, 2020 11:52 pm Is it as simple as using the Helix operation . . .
Josh,

I believe the existing helix operation would be unsuited. It adjusts the spiral pitch to match the depth of the hole, giving an integral number of turns. That would not be cool for threading. It probably could be massaged to work with some fairly small code changes.

I suspect that chrisb's suggestion would be quite a lot of work. In this case I would stay away from interpreting solid models and just use something simple to create the required g-code.

I have seen simple thread-mill code generators on the internet, but it would not be difficult to write the code by hand.

Gene
chrisb
Posts: 37776
Joined: Tue Mar 17, 2015 9:14 am

Re: thread milling?

Post by chrisb »

GeneFC wrote: Thu Aug 20, 2020 3:08 pm I suspect that chrisb's suggestion would be quite a lot of work. In this case I would stay away from interpreting solid models and just use something simple to create the required g-code.
You are probably right. Path has already a hole detection mechanism. With a simple probability to enter the pitch and possibly the thread diameter is may not be too difficult to add thread cutting helix code.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
User avatar
dubstar-04
Posts: 660
Joined: Mon Mar 04, 2013 8:41 pm
Location: Chester, UK
Contact:

Re: thread milling?

Post by dubstar-04 »

mlampert has done most the work for a thread milling op:

https://github.com/mlampert/FreeCAD/tre ... ad-milling
RatonLaveur
Posts: 990
Joined: Wed Mar 27, 2019 10:45 am

Re: thread milling?

Post by RatonLaveur »

Most online jobshops receiving a step file and providing a quote (protolabs, weerg... there's a plethora) have a thread detection system based on hole diameter.

The holes produced in Part Design can be specified threaded, in which case the nominal diameter in the model is automatically the necessary drilling diameter with material allowance for the tap to do its work.

It would be quite adequate to use a similar UI as that used by the PartDesign hole tool to select a threading method.

That being said i may be off with regards to your request as you seem to be interested in thread milling, in which case i would suggest a drop down menu with ISO standards for example that produce automatically the correct helix...but the tool diameter and threading type (coarse or fine) needs to be taken into account.
User avatar
<Charlie_root>
Posts: 53
Joined: Mon Aug 12, 2019 8:01 pm
Contact:

Re: thread milling?

Post by <Charlie_root> »

I didn't even know it was possible to make threads with a helical path

I assumed you needed a tap for that size hole and use a drill operation
you also needed a collet with Z-play in order to do this
RETRIBUTION IS AT HAND
User avatar
JoshM
Posts: 456
Joined: Thu Oct 05, 2017 5:34 pm
Location: New Hampshire

Re: thread milling?

Post by JoshM »

So, there are various ways this is done, including what you describe, which uses a clutch to drive a tap for internal threading. Generally they are pricey, by hobbyist standards. $500-$1000 range likely.
Image

The method I was suggesting uses the tool image I linked and that tool is sized for a certain pitch. The tool is effectively a 60-deg trapezoid, with several reliefs that are the cutting edges. When the rotating tool is fed along a right or left hand helix, matching the pitch, it cuts the threads. This might be done in multiple passes, each moving towards the final radius, depending on the job.

What I like about this method in concept is that it makes it easier to ensure that the threads are orthogonal to the milled/drilled hole, and thus the face. I'm horrible at hand drilling or threading or anything requiring a steady hand or requirement for a 90 or 45 degree angle.

The reason the tool is tied to pitch is that the calculation for the trapezoidal thread requires Dmin, Dmaj, P, and H, and 60-deg., where P is pitch, and H, which equals SQRT(3/4) x P, about 0.866 x P. This means that the radial cut equals 3/4 x H = 3/4 x 0.866 x P, which I believe is why the course/fine pitch values increase as the D decreases.

Image
tigr180
Posts: 4
Joined: Thu Oct 08, 2020 3:37 pm
Location: Taiwan

Re: thread milling?

Post by tigr180 »

Hello,

it is my first visit to the forum. So I make a comment, hopefully worth reading.

Pros for thread milling:
  • it is not required to have a cutter for each thread, odd type threads are possible. e.g. M80x0.45 or multi start threads.
  • Spindle speed control is not critical
  • Spindle position is not definded
  • Very low torque requirements compare to tapping
  • If the thread mill breaks inside a hole it usually can be removed
Cons for thread milling:
  • tool deflection plays a big role when thread milling e.g. in steel. Very tedious to dial correct diameters and other parameters in. Seems that several trial cuts on a scrap part are adviseable.
  • If the machine is not very acurate it can quickly become soso, 0.1mm backlash on e.g. y-axis can spoil a thread quite a bit.
  • Unfortunately the threadmills are quite expensive compared to smaller machine taps. Both break easy :-(

Whishlist, from another "nothing programmer", "just whisher".
  • thread milling can be also done for outside threads, so it would be nice to have that option also for outside of a cylinder?
  • There are thread mils with one tooth, or multiple tooth. Multiple tooth can only do one pitch and require less circles to cutt the complete thread. Also tool diameter and thread form are not necessary a fixed combination. Some way of linking path output with tool properties would be excellent.
  • overall diameter and pitch are basically independent, so a M80x0.45 would be possible. Or any of these weird imperial threads, even threads with 55° angle are doable. When using the right cutter.
  • somehow it should be possible to do several passes with different diameters to get chip load reasonable
  • nice to have an option for spring passes?
  • multiple start threads
  • tapered threads,
  • automatic detection and all in one automatic would be the "killer-app", but very scifi
User avatar
sliptonic
Posts: 2445
Joined: Tue Oct 25, 2011 10:46 pm
Location: Columbia, Missouri
Contact:

Re: thread milling?

Post by sliptonic »

This is another awesome feature that I would like to see in Path. But like others, It's tough to get developers (or myself) interested in doing it without hardware to test on.

Does someone have access to thread mills? If someone can provide thread mills or sponsor a developer to buy one, it's much more likely that this will see the light of day.

Do you work commercially and know a tooling manufacturer representative? Tell them you want to use FreeCAD and ask them to donate tools or money to make it happen.

Do you have a twitter account? Tweet at manufacturers and ask the same thing. Very often manufacturers have customer returns or manufacturing prototypes that they can't sell. Sometimes it's just a matter of asking.
Post Reply