Thread Cutting?

This forum is for general discussion about Aspire

Thread Cutting?

Postby Posthill » Tue Mar 16, 2010 3:52 am

Hi Guys,

The other day I was making a new dust collection housing for my router because the other one was not working very well. Anyway I bought a 1.5" threaded plumbing fitting but of course I had no way to cut threads that big so I started playing in Aspire and using the Profile Tool Path added a spiral ramp to the toolpath that was going to cut my circle out. Then set my tool up so that it only was able to plunge the amount of depth that I wanted for each thread. I found I could actually set up how many threads per inch I wanted with this arrangement. My biggest problem after that was to find a tool that would cut the thread properly. I looked online for something suitable and couldn't find anything. I ended up using a .500' dovetail bit and was able to cut a haphazard thread with it and the fitting actually tightened up fine. I have some other ideas for projects that I's like to cut threads into but I'd rather not use the dovetail as it really doesn't do the job well.

Does anyone know of any tooling available that would be able to cut a thread on its outer radius or have another method to cut threads in somewhat large holes?

JP
Jeff Postma
Aspire User
www.posthill-innovations.com
Bracebridge, Ontario, Canada
Posthill
Vectric Apprentice
 
Posts: 59
Joined: Tue Sep 08, 2009 12:45 pm
Location: Bracebridge, Ontario, Canada

Re: Thread Cutting?

Postby RoutnAbout » Tue Mar 16, 2010 4:51 am

Does anyone know of any tooling available that would be able to cut a thread on its outer radius or have another method to cut threads in somewhat large holes?


Jeff,
I can't seem to find the websites that I thought I had bookmarked.
I just did a search and came up with this site that sells thread mills. Hang on to your chair when you see the prices. There are cheaper thread mills, I just need to look harder.

What I've done in the past is to take a Keyset cutter or Woodruff keyset (one with straight flutes - not one with staggered flutes) and then grind a 30° chamfer on the top and bottom to create the thread form.
Hope that helps.
Roll of Honor <-- Never Forget
________
Don
User avatar
RoutnAbout
Vectric Wizard
 
Posts: 2058
Joined: Mon Sep 19, 2005 11:09 pm
Location: North Manchester, Indiana
Model of CNC Machine: Old Bot with a Rope Pull Start Spindle

Re: Thread Cutting?

Postby Woodmolds » Tue Mar 16, 2010 12:53 pm

Might this be the type bit you're looking for?
http://magnate.net/index.cfm?event=showProductGroup&theID=119


Tony
Working with wood as a profession, since 1972.
User avatar
Woodmolds
Vectric Craftsman
 
Posts: 106
Joined: Mon Apr 06, 2009 12:05 am
Location: Piedmont, North Carolina USA

Re: Thread Cutting?

Postby RoutnAbout » Tue Mar 16, 2010 12:59 pm

Woodmolds wrote:Might this be the type bit you're looking for?
http://magnate.net/index.cfm?event=showProductGroup&theID=119
Tony


Thanks Tony, that will work. I need to bookmark that site.
Roll of Honor <-- Never Forget
________
Don
User avatar
RoutnAbout
Vectric Wizard
 
Posts: 2058
Joined: Mon Sep 19, 2005 11:09 pm
Location: North Manchester, Indiana
Model of CNC Machine: Old Bot with a Rope Pull Start Spindle

Re: Thread Cutting?

Postby Woodmolds » Tue Mar 16, 2010 5:59 pm

Here are some more with 60deg angle.

http://www.harveytool.com/products/index.php?page_function=show_family&product_family=Double+Angle+Shank+Cutters&category_id=1

http://www.use-enco.com/CGI/INPDFF?PMPAGE=119&PMITEM=619-1390

I would also be very interested in how to accomplish this(internal treads) if anyone is willing to share!
Working with wood as a profession, since 1972.
User avatar
Woodmolds
Vectric Craftsman
 
Posts: 106
Joined: Mon Apr 06, 2009 12:05 am
Location: Piedmont, North Carolina USA

Re: Thread Cutting?

Postby Posthill » Tue Mar 16, 2010 6:33 pm

Thanks so much guys!!! When I did a search for thread cutting tools all I got was reams of how to's on a lathe. Love this forum! :mrgreen:

JP
Jeff Postma
Aspire User
www.posthill-innovations.com
Bracebridge, Ontario, Canada
Posthill
Vectric Apprentice
 
Posts: 59
Joined: Tue Sep 08, 2009 12:45 pm
Location: Bracebridge, Ontario, Canada

Re: Thread Cutting?

Postby RoutnAbout » Tue Mar 16, 2010 6:36 pm

Tony,
I don't think this can be acheived with this software.
But my control software allows me to cut a circle from the keyboard, with option of the following parameters:
Code: Select all
CG Command :  diameter, X-end-point, Y-end-point, *X-center-offset(I), *Y-center-offset(J) {,[O]ut-[I]in-[T]rue, direction, plunge, repetitions, proportion-X, proportion-Y, [1-TAB feature ON; 2-POCKET feature ON; 3-SPIRAL feature ON; 4-SPIRAL & Bottom Pass feature ON], 1-no pull up at end, 1-do plunge from Z-axis 0}


This allows me to cut a circle and a given it a diameter, and to spiral down at a given rate and distance. And by using the formed tools you've posted will cut the thread your asking for.
I'm don't have access to my router or vectrics software right now, but will take a look at the profiling of a circle. Give me 3-4 hours and I'll be able to look and see if its possible.

Tim might jump in here and post this info before I can get access to aspire.

Thanks so much guys!!! When I did a search for thread cutting tools all I got was reams of how to's on a lathe. Love this forum! :mrgreen:
JP

Jeff, Glad to help
Roll of Honor <-- Never Forget
________
Don
User avatar
RoutnAbout
Vectric Wizard
 
Posts: 2058
Joined: Mon Sep 19, 2005 11:09 pm
Location: North Manchester, Indiana
Model of CNC Machine: Old Bot with a Rope Pull Start Spindle

Re: Thread Cutting?

Postby RoutnAbout » Wed Mar 17, 2010 1:29 am

I think I may have figured out how to cut Threads on any size diameter circle.
All one has to do is figure out how many threads you need in the thickness of the material.
Divide your material thickness by the number of thread, this will give you the cut depth per pass.

In this example the material is 1" thick
Toolpath on left 4 revolutions or threads in 1" material.
Toolpath on right is 1 revolution or thread in 1" material.

I'm sure this will work with the tooling post above.
I hope this helps and might find this useful.
Attachments
Sprial Threading.jpg
Spiral Ramping.jpg
Roll of Honor <-- Never Forget
________
Don
User avatar
RoutnAbout
Vectric Wizard
 
Posts: 2058
Joined: Mon Sep 19, 2005 11:09 pm
Location: North Manchester, Indiana
Model of CNC Machine: Old Bot with a Rope Pull Start Spindle

Re: Thread Cutting?

Postby tmerrill » Wed Mar 17, 2010 1:42 am

One hiccup will be the inability to use lead-ins and outs with the spiral toolpath. So when you get to the bottom of the hole the bit extracts straight up which will leave a vertical cut the same depth as the threads in the side.

In some applications this probably won't matter, but if it does the only solution I see is to edit the toolpath and manually add a move to the center of the hole before the bit pulls out.

It will also take a little math work for the setup because everything is being calculated from the center of the bit. I would think one would have to figure out what depth threads are wanted and then offset the toolpath inwards to adjust. Not hard to do, but the actual steps would probably depend on the bit design and dimensions.

Very interesting, I hope someone does some samples and posts the results.

Tim
tmerrill
Vectric Archimage
 
Posts: 4794
Joined: Thu May 18, 2006 3:24 pm
Location: North Carolina
Model of CNC Machine: ShopBot

Re: Thread Cutting?

Postby RoutnAbout » Wed Mar 17, 2010 1:48 am

Good Catch Tim,
I was thinking out I do it on the Bot, and the control software takes care of this.
Back to the drawing board :)
I suppose one could toolpath this with a slow feed rate and use stop or pause (unless your system pulls up the tool)
Roll of Honor <-- Never Forget
________
Don
User avatar
RoutnAbout
Vectric Wizard
 
Posts: 2058
Joined: Mon Sep 19, 2005 11:09 pm
Location: North Manchester, Indiana
Model of CNC Machine: Old Bot with a Rope Pull Start Spindle

Re: Thread Cutting?

Postby tmerrill » Wed Mar 17, 2010 2:07 am

There is an easy solution - buy Brian a pint or two or three and ask for a threading gadget :D
tmerrill
Vectric Archimage
 
Posts: 4794
Joined: Thu May 18, 2006 3:24 pm
Location: North Carolina
Model of CNC Machine: ShopBot

Re: Thread Cutting?

Postby RoutnAbout » Wed Mar 17, 2010 2:13 am

tmerrill wrote:There is an easy solution - buy Brian a pint or two or three and ask for a threading gadget :D --- Hey Brian ====>>> it was Tim that made the suggestion
Roll of Honor <-- Never Forget
________
Don
User avatar
RoutnAbout
Vectric Wizard
 
Posts: 2058
Joined: Mon Sep 19, 2005 11:09 pm
Location: North Manchester, Indiana
Model of CNC Machine: Old Bot with a Rope Pull Start Spindle

Re: Thread Cutting?

Postby BrianM » Wed Mar 17, 2010 9:51 am

RoutnAbout wrote:
tmerrill wrote:There is an easy solution - buy Brian a pint or two or three and ask for a threading gadget :D --- Hey Brian ====>>> it was Tim that made the suggestion


I have obviously managed to develop a reputation for being pretty cheap ... :D

Seriously, machining threads seems a pretty specialised area which I don't think many people are doing. Any gadgets need to have a reasonably wide appeal to justify development effort.

Brian
User avatar
BrianM
Vectric Staff
 
Posts: 1754
Joined: Mon May 16, 2005 10:15 am
Location: Redditch U.K

Re: Thread Cutting?

Postby tmerrill » Wed Mar 17, 2010 10:33 am

Brian,

Don says he is disappointed, but understands, and will still buy you the beers :D
tmerrill
Vectric Archimage
 
Posts: 4794
Joined: Thu May 18, 2006 3:24 pm
Location: North Carolina
Model of CNC Machine: ShopBot

Re: Thread Cutting?

Postby kilrabit » Wed Mar 17, 2010 11:06 am

If you have mach3 it has a threading wizard that works very well, I use the same kind of threading tool.
kilrabit
Vectric Wizard
 
Posts: 465
Joined: Thu Feb 26, 2009 4:04 am
Location: Uvalde Texas

Next

Return to Aspire - General

Who is online

Users browsing this forum: No registered users and 3 guests