Cutting threads

[gugnheim]

Has anyone done any thread cutting work with their indexer? I don't own one yet, but in the course of thinking of projects this came to mind from my workbench screws. They are getting on needing replaced and if I recall, about 2 tpi and 2 inch dia.
Thanks
Ryan

[myxpykalix]

here is a discussion in another forum:
http://www.vectric.com/forum/viewtopic.php?f=27&t=8074

[dana_swift]

Cutting threads is a capability I want too.. been kicking around writing a toolpath generator for the task, haven't gotten around to it yet.

I want to be able to cut inside and outside threads, and have figured out how I will tackle the task when the time comes. Also I have thought about optics-standards threads for C mounts, CS, filters, etc.

Also want to be able to make pipe-threads as well as straight machine screw threads.

Should be an interesting project- now to get the time it requires-

D

[billp]

Guys,
Check out the picture of the threading work done by Todd Maci on the Camp Flickr page- http://www.flickr.com/photos/campshopbot/3959948069/in/set-72157622468368762/
If you can't make that link work go to the thread for the 2009 Mystic, CT Camp- http://www.talkshopbot.com/forum/showthread.php?t=2099 and follow up the link to the pictures....

[gugnheim]

Very cool! That's exactly what I am talking about. Ways to rebuild parts on my Roubo style workbenches when I do oops things...
Ryan

[donchandler]

You don't need a indexer to cut threads. Cut a hole in your table and make a support under it. Clamp your bar stock to the support so the bar is vertical. Let the bar stick up above the surface of the table. I center on the bar and then use a 1/2" bit to run around the bar to make sure it is round and to get it to a exact size. Put in a thread milling cutter and use the CP command to spiral down at the pitch you want and for the number of turns. You thread holes the same way. You have to figure out the offset for the threading cutter to get the tread depth right. I have done threads from 3/4" up to 24" dia this way.
I do pipe threads the same way, but I have to make a tapered tool path in CAD-CAM.

[widgetworks_unlimited]

Compared to cutting a lot of other less complicated shapes, the tool path for cutting outside threads on the indexer is surprisingly simple...

&Cut_Depth_Start = 1
&Cut_Depth_Finish = 2 'Same as Start for straight threads
&Thread_Pitch = 20
&Thread_Length = 5

M5, X,Y,Z,,B 'Move spindle above start point of thread
MZ, &Cut_Depth_Start 'Move Z down to cutting depth at start of thread

'Cut thread - either straight or tapered
&Rotation_Degrees = &Pitch * &Thread_Length * 360
M5, ,&Thread_Length,&Cut_Depth_Finish,,&Rotation_Degrees


Note - the example above is for indexers that are parallel to the Y axis. For X axis indexers, swap the following in place of the last line shown above...

M5, &Thread_Length,,&Cut_Depth_Finish,,&Rotation_Degrees

[dana_swift]

Russ, the elegance of your solution is wonderful.

Well done!

Suggestion.. put some input boxes to allow run-time entry of the parameters..

D

[widgetworks_unlimited]

Thanks Dana - I wrote that code on the fly, just to show how simple it was. When I first built our indexer I wrote a bunch of automated programs for creating blanks and simple profiles. I was amazed at how shapes that are hard in 3-axis are simple in 4-axis and also the other way around.

While PartWorks 2.5 is great with some 4th axis work, some simple operations are much easier to create the "old fashion way". Code that's written to leverage 4th axis abilities (instead of wrapping 2.5D/3D) can be cut in a fraction of the time.

I agree with you - if I were to use the code, I would probably add a few input/message boxes.

You mentioned that you've got a method for cutting inside threads? Are you planning to cut them with a tap in the tail stock? I haven't found another way to use the ShopBot for this type of opperation. I had played around with the idea of adding gang lathe type attachments to our Z-axis, but with all the unknowns about rigidity, accuracy, stress/wear, I ended up just buying another metal lathe that I'm converting to CNC control. With our metal lathe we can use a boring bar style cutter for inside work.