Thread cutting

[crpoj13]

If anyone is interested in seeing the video please check out my instagram account- mrjasonowen

[Bobtail Farm]

crpoj13:
thanks,
Brian.

[Tailmaker]

I continued playing with the threads and found that the fluting toolpath provides a real good solution, no g-code editing or gadget required (the flute ramps linearly over the entire length). I made a spreadsheet to calculate the sweep angle and depth of the thread arc fluting cuts for the Magnate threading bit (makes 90 degree v-shaped threads) and also for a 1/2"dia 3/16"wide keyhole bit (makes a kind of ACME thread). The latter is a bit more complicated calculation since the bit attack angle makes the thread sides become tapered but it works very well. With ~0.01" specified clearance gap the "bolts" go in smoothly.

For the examples below I made a 4-start thread for the keyhole bit and an 8-start thread for the Magnate bit. Of course a regular single start thread is possible as well.

For ACME threads:

FluteThreadingKeyhole.crv3d

(584 KiB) Downloaded 147 times

FluteThreadingKeyhole.crv

(577.5 KiB) Downloaded 138 times

[crpoj13]

Tailmaker this is pretty neat. Any chance of sharing spreadsheet?

[Tailmaker]

Tailmaker this is pretty neat. Any chance of sharing spreadsheet?

I could do that but I guess I would need to make it more understandable for other users. Let me see what I can do.

The key for using the fluting tool path is to add short "dog legs" (length equal thread cutting depth) to the beginning and end of the thread arc to clear the thread when retracting. The spreadsheet adds this length to the total arc length to cacluate the proper flute depth. It is the reason why the flute cutting depth is slightly different for the male and female thread with the same pitch.

Drawing the thread arcs is easy in Aspire/VcarvePro when they are less than 360 degrees (draw a circle and cut out the required angle). It becomes more interesting to make an arc vector larger than 360 degrees. But even that is easy, example here an arc of 937 degrees: Divide 937 by 3 (or whatever is needed to get the result under 360) and draw the resulting arc of 312.333 degrees. Then use the circular copy function to make 3 of them also spaced 312.333 degrees apart, making the total angle 937 degrees again. Then join them together (Aspire does not care that it has several loops in one vector on top of each other). Identify the start point and the end point in Node Editing mode and add the above mentioned "dog legs". Depending on which vector end is the start point it will become a left or right hand thread. For multi-start threads, this complete vector can also be circular copied as many times a needed (180 degrees for 2-start, 90 degrees for 4-start etc.). Once you have the numbers it takes only short time to create the tool paths.

The ACME thread has actually a little more backlash; I believe this is because the squarish keyhole cutter makes a slightly different profile in the male and female threads. It also means for the ACME thread the "bolt" diameter should be at least 5 time the cutter diameter.

Both thread types can take a lot of load and could be used e.g. in height adjustment features. The specified gap in the spreadsheet may have to be increased, depending on the accuracy of the CNC machine.

[Tailmaker]

Tailmaker this is pretty neat. Any chance of sharing spreadsheet?

I started a new thread with links to the spreadsheet download: http://forum.vectric.com/viewtopic.php?f=28&t=30624

[Bobtail Farm]

Way cool. In awe.

[crpoj13]

I look forward to giving this a try, thanks for sharing!