blind dove tails on cnc

This is the place to post images of work produced using Aspire
john teichman
Vectric Apprentice
Posts: 81
Joined: Fri May 19, 2006 8:30 pm

Re: blind dove tails on cnc

Post by john teichman »

john teichman wrote:
john teichman wrote:Hi James i have a 1.75 overhang on front so should be able to do around 48in one pass. for this i use 1.25 off set on y and 2.5 on x i dont have a clamping method yet just screws for now. i will send file for .5 blind maybe some one can improve on them.John, sorry forgot: profile cut outside .50 deep .375dia. 14 deg dove cutter use only 25 in pm @ 12000 rpm i use .375 end mill for tool path but actually use dove tail cutter instead.
James sorry the cut depth should have been .375 i am working on through dove tail @ same time.
Hi again i played w/ through dove tails today i will post crv. files, they can be made real tight but the tear out is bad, maybe some one will improve or redo. i ran @ 25 ipm and 12000 rpm
Attachments
winter 08 around christmas 498.jpg
dove tail tails .5 end mill .5 mat..crv3d
(64.5 KiB) Downloaded 617 times
dove tail pockets 14deg. .5 cutter .5mat..crv3d
(57.5 KiB) Downloaded 539 times

madtownrob
Posts: 34
Joined: Mon Mar 09, 2009 7:03 pm
Location: Madtown, Wi

Re: blind dove tails on cnc

Post by madtownrob »

I have been a lurker for some time here and I have also been working on dovetails on the my CNC due to the posts on shopbot as well as the psost I have been reading here. Thanks for the inspiration!

I have a Joe's Hybrid4x4 and have been cutting box joints and dovetails with some good success. I have programmed to tool path to first climb cut then to clear out the waste. I have no tear-out when I do this. I have posted a short video of a box joint I have been using for multiple boxes:



I have also been cutting some dovetails using the same process of a climb cut first
Pins:
dt3.JPG
pins 2
pins 2


Tails:
tails1
tails1
dt2.JPG

This was a test at slow feed rates to see how well it did. Nice and tight, no tearout. I will need to due some toolpath optimization on this one to get it to cut faster, but happy with th result anyway

Also cut some "curvey" dovetails that cam out pretty decent - tight enough that the dry fit took some persuasion to get apart :). I need to play with the toolpaths and first cut a small climbcut on the ends of the boards to prevent tearout - it was pretty bad!
assembled
assembled
curvy1
curvy1

Thanks for looking!
- Rob

cabnet636
Vectric Wizard
Posts: 2596
Joined: Fri Dec 21, 2007 1:57 am
Model of CNC Machine: CAMaster 508 ATC
Location: columbia sc
Contact:

Re: blind dove tails on cnc

Post by cabnet636 »

rob you are the man!!

jim
James McGrew
http://www.mcgrewwoodwork.com
CAMaster ATC 508 24/7 http://dropc.am/p/EJaKyl

User avatar
juan
Vectric Apprentice
Posts: 93
Joined: Tue Aug 15, 2006 10:55 am
Location: The Netherlands
Contact:

Re: blind dove tails on cnc

Post by juan »

Very good Rob,

I may say that as an carpenter :wink:

Did you made that toolpath with aspire?
Or did you make it by hand?

Great job Rob,

Juan

madtownrob
Posts: 34
Joined: Mon Mar 09, 2009 7:03 pm
Location: Madtown, Wi

Re: blind dove tails on cnc

Post by madtownrob »

Jim thanks I follow your work over at SawmillCreek - lots of inspiration for me -


Juan - I started out making the outline of the vectors in AutoCAD. It is just easier for me to draw things exactly how I want them looking on the vertical end of the board. I first decided on a dovetail and straight bit size (7degree 0.5" dia Dovetail and a 0.50 inch End Mill) for the pins and box joints. looking down on the board end, I draw a dovetail with 7 degree sides and the wide diameter of the 0.5" dimension. I make this dovetail .75" tall (my wood thickness) I create a block of this part to be able to copy it again.

I now draw the end view of my board .75" tall x 8.25" wide in the examples. I make two copies of this rectangle - 1 on top of another separated in the Y by a few inches. I copy the dovetail block to have it an overhang on both sides, then split the difference twice - this gives me 5 dovetails. I then use this to project the center lines of the individual dovetails down to the other 0.75"x8.25" board. I suse thes line to create a "ON PROFILE" tool path. I just draw a vector starting where I want and trace the exact path I want the dovetail cutter to follow (full pass depth = Board Thickness)

For the Pin Board (I extend the sides of the dovetails out and additional 1/2 of the bit diameter + 1/8" for clearance on both the top and bottom. I then trace the outline of a "PROFILE OUTSIDE" Tool path to cut the climb cuts at full depth. I next create pockets of this the area to be cleared and create pocket tool paths of the closed vectors.
Capture-1.jpg
It really is simpler than it sounds. I have attached a DXF. The big thing is to try and draw a vector that will either be machined on or on one the outside. You have to make your own clearance assumptions. If you have any other questions please cask. Thanks!
Attachments
8 qrtr dovetail 7 deg bit.dxf
(123.21 KiB) Downloaded 664 times
dovetails -pins.crv3d
(107.5 KiB) Downloaded 557 times
dovetails -tails.crv3d
(73 KiB) Downloaded 493 times

cabnet636
Vectric Wizard
Posts: 2596
Joined: Fri Dec 21, 2007 1:57 am
Model of CNC Machine: CAMaster 508 ATC
Location: columbia sc
Contact:

Re: blind dove tails on cnc

Post by cabnet636 »

this is way too cool!!!

jim
James McGrew
http://www.mcgrewwoodwork.com
CAMaster ATC 508 24/7 http://dropc.am/p/EJaKyl

User avatar
IslaWW
Vectric Wizard
Posts: 1402
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: blind dove tails on cnc

Post by IslaWW »

Guys...
Here are our segented (FJ) Birch economy and Solid Maple standard drawer boxes. Cut on ShopBot PRSa @ 1.25 ips using a 5/8 dia, 14 degree bit @ 12K rpm. Cutting time for the 10" boxes is about a minute and another for load and unload. 14 drawer boxes complete in under 30 minutes.

Cutting is accomplished by entering widths and thickness' of material as variables into running cutting file that makes all calculations. Options are given to adjust the slot length or cut depth so that near perfect fit is always easy.
Attachments
DSC01765cmp.jpg
DSC01766cmp.jpg
DSC01767cmp.jpg
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

moto633
Vectric Wizard
Posts: 1123
Joined: Sun Jul 13, 2008 11:59 am
Location: Rockbridge, Ohio

Re: blind dove tails on cnc

Post by moto633 »

Gary that is awsome!!

Now I really need to figure out the jig setup. Could you post more detailed pics of your jig???

I have the basic idea but would like to see all sides of it if you have the time.

Thanks,
Nick

User avatar
IslaWW
Vectric Wizard
Posts: 1402
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: blind dove tails on cnc

Post by IslaWW »

Nick....
All the pics I have and building details are here: http://www.shopbottools.com/garysmusings.htm#Dovetail Jim McG is the proud new owner of that jig. (extorsion) :D I now use the same air clamp system, with a diferent orientaion index, as I do for doweling: If you have any specific questions email me, put dovetail in the subject line.
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

cabnet636
Vectric Wizard
Posts: 2596
Joined: Fri Dec 21, 2007 1:57 am
Model of CNC Machine: CAMaster 508 ATC
Location: columbia sc
Contact:

Re: blind dove tails on cnc

Post by cabnet636 »

gary i have really enjoyed our conversations and your videos, my cabnetware is designer and is the step before detailer which was the cutlister program so no csv file
should get the jig tommorrow as we were in and out all day
jim
James McGrew
http://www.mcgrewwoodwork.com
CAMaster ATC 508 24/7 http://dropc.am/p/EJaKyl

endgrainguy
Vectric Apprentice
Posts: 82
Joined: Tue May 20, 2008 9:09 pm
Location: Colrain, MA USA
Contact:

Re: blind dove tails on cnc

Post by endgrainguy »

As part of an exchange I"ve had with Paul as a result of this thread, who's working on a spread sheet approach to dovetailing:
(See examples of my work at http://www.alladd.com)
I"m attaching examples of how i do my dovetails, both through and half blind.
About my machine - it's a shop built machine I designed and made last year, using high quality components bought off Ebay -THK type rails, ballscrews, 20-20 extrusions and aluminum plate. Its fixed gantry, moving table, with 32 inches of x travel, and a table that moves 20" for y. I built it so that the table can be positioned at the end of a bit with the router tilted horizontally, for dovetailing and mortise and tenon work. The end of the laminated plywood worktable is t-slotted so lipped extensions can be easily bolted on to serve as stops, and also as backer to prevent tear out. The horizontal work position greatly simplifies clamping. For wider work, (which for me is anything over 1.5") I use vacuum hold-down from a compressor venturi using gasket placed in a grid of grooves machined into my table, along with the usual Shopfox cam clamp that's sufficient clamping alone for narrower work. I run the machine at about 50 IPM x and Y and 30 IPM Z. For joinery work, I"ve defined a version of mach with y and Z reversed, so I can draw a part in the usual way and cut it with my horizontal router. The drawings I"m attaching are for that version of Mach. I initially used a Bosch 12 amp router, but a few months ago swapped it out for one of the inexpensive Chinese water-cooled spindles, which saves a great deal of noise, and doesn't bog down on heavy cuts.
My process is to start by copying the "copyablevectorset" and paste it into a new v-carve file of the correct size. These vectorsets are really analogous to the fingers in a Leigh router jig, in that they define the spacing between tail cuts and their adjacent pin cuts. I have a copyable vectorset for each bit, and they can cover a range of stock thicknesses, and are easily altered for thicker or thinner stock. I usually center the first set, then paste additional copies and space them as desired. The slanted vectors are simply joined and closed to form boxes that will cut the pins by profiling on the inside of the box. If the tails are large enough they may require an additional cut in the center to remove all pin waste, but judicious bit selection and vector formation should keep that from being necessary, at least for stock thinner than .5", (thicker if one uses large straight bits rather than the preferred spirals) and that saves a lot of work if one wants the best possible router time economy. Note that my method cuts half-way through from each side with the dovetail bit for the tail cuts, eliminating tear out. This allows me to index the work on the bit itself, without requiring a backer or other stop for positioning the work. The code for tails then starts with a safe z move, and cuts the tails by first scribing the ends of the stock with a light climb cut( see the vectors for these in the 1.8 inch through dovetail drawing) and then cuts the tails half way from above, and then comes around and meets the cuts from the bottom. If using delicate bits I will prekerf with another tool (as in tablesaw or bandsaw.This can be done very quickly.) . I remove the extraneous z moves manually after checking the cut on scrap, or just in the air. I can fine tune the fit after cutting sample pins by changing the 0 setting on my y axis (the usual z axis). Two inch wide parts are machined in well under a minute each, and I often have a router table set up near by, to cut grooves for bottoms , to keep me busy while the dovetails are cut, so my time cutting them is really only that required to clamp and unclamp them.
I have less experience with half blinds, as through dovetails are so much easier to cut by virtue of the excellent cut one gets with solid carbide spirals, that I now use through dovetails in some applications I formerly used half blind. The half blinds are done in a similar fashion, using the half blind vector set I attach an example of. The pins are cut with a dovetail bit with the router in the usual position, and fit is controlled with great precision, if necessary, by using the profile allowance offset function.
Feel free to let me know if you'd like clarification of any of this.
It seems like a spread sheet approach would be faster for someone doing lots of different sizes in small numbers, and I eventually would like to go over and figure out your method, and the logic you used to generate it. I've known that something like an "insert these few numerical parameters and generate g-code " algorithim was possible, and now i see fundamentally what it looks like. Thanks so much for your work, and for sharing it! Best, Al
Attachments
2.25 silvercjhestINCHHALFBLIND.crv
(37.5 KiB) Downloaded 580 times
NEWcopyablecentervectorsetfor.187dovetail,5.crv
(24.5 KiB) Downloaded 543 times
2.25 inch.crv
(32 KiB) Downloaded 547 times
I thought this was supposed to make life easier?

Post Reply