Yesterday I 3D printed this secret box to insert a gift for my granddaughter birthday. I was wandering how I could do it on my CNC with hardwood. I think the only way is to have some special cutter. Any suggestion?
Here are the sty file link on thingiverse:
Thanks,
Robert
You could do this with a dovetail bit easily enough. Just need to plan your paths so all your plunges and retracts are outside your piece.
The angles won’t be as steep, but other than that would work the same way.
https://www.leevalley.com/en-ca/shop/tools/power-tool-accessories/router-bits/30172-dovetail-bits
Hi Micheal, I though of that too, but I think with this kind of angle, the aspect of the box won’t be has nice. I still may try it, will have to redesign and may 3d print it for a test, thanks.
Unfortunately, Carbide Create won’t correctly preview a dovetail tool, see:
The secret of the impossible dovetail is they are at an angle. So make multiple tool paths. Cut the widest part of the female dovetail with a flat end mill to remove the majority of the waste. Then make the dovetail cut at full depth with a longer tool path than the actual size of the dovetail. You want to plunge in outside of the cut and retract outside of the cut. I think the project is doable but will take some planning and consideration. You might want to use the painters tape and superglue workholding so clamps are not in the way. I have an L bracket I use to set up the material so it is square with the cutter, put the tape and super glue down and then remove the L bracket.
Do the same thing for the male part of the dovetail, remove the majority of the material with a flat end mill and make a full depth cut with the dovetail bit.
You cannot make incremental cuts with the dovetail like a pocket but you can move the dovetail bit over at full depth and then make incremental cuts at full depth till your dovetail is completely formed.
You can always make one by hand 
Will, for this kind of project I would use Fusion360.
Guy, I would use a similar process too but dovetail router bit have a quite different angle, 7 to 14 degrees angle, much different than this model. With google, I found some similar wooden boxes all with the same angle and they are at low prices. They must use some jigs on the table saws?
Nick, thanks for this video, interesting! Wandering if the change in humidity thru seasons will affect the operation. Would not think doing those kind of work by hands, not enough skills and patience!
Simple enough to do in OpenSCAD:
https://www.blockscad3d.com/community/projects/1424448
It’d be pretty straight-forward to take the model and cut it w/ a dovetail tool which matches what is entered into the parameters.
Thanks Will, I am not familiar at all with BlocksCAD neither OpenSCAD, but I will look at it and I have a good friend who is familiar with OpenSCAD, he will help me.
Really wish it was straight-forward getting DXFs suitable for cutting out of OpenSCAD — for one approach see:
Drawing up the design in Carbide Create is pretty workable:
Draw a square for the outline of the box:
Rotate 45 degreees:
Draw up the dovetail tool in profile:
and draw in a rectangle to measure the width of the dovetail slot:
Draw in a square to get the size:
scale by 0.5 to get half:
and reposition:
Select the rectangle for the pocket and align it:
Then increase the size as necessary to cut away completely:
and draw in a straight line along the center:
copy-paste the line and the rectangle into place so as to duplicate them:
Then select the rotated rectangle and flip horizontally:
Draw in the dovetail tool to verify that it will clear:
and if it doesn’t, increase lengths so that it does:
Rotate everything back:
and assign toolpaths:
As noted, you won’t get a correct preview:
You’ll also want to draw in a pocket so that it will serve as a box rather than a puzzle, and add either a ball-catch or magnet.
An elongated pocket increases the storage volume:
Duplicate the file and adjust as necessary to cut the negative of the dovetails so as to make the lid.
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.
For folks who don’t have OpenSCAD installed it is available at:
Click on the icon for “Customizer”
to adjust things and choose “DXF” rather than STL to be able to export a DXF or SVG:
EDIT: Note that the image below shows an incorrect construction caused by an error (since corrected) in the OpenSCAD code — adjusting for that error (and finding it in a check of the files) is shown below.
which may then be loaded into Carbide Create:
to have toolpaths created.
The geometry will be used as guidelines in creating the geometry and toolpaths needed to actually cut out the design.
The actual box outline will be rotated 45 degrees:
to make it easier to arrange the stock on the machine to cut — the other elements will be brought into alignment with it.
Done
Since Carbide Create cannot show undercuts in the 3D preview, we will draw up the Dovetail tool in profile, and use a proxy circle for it to check at need.
The basics of the box are quite straightforward:
as per usual we offset to the outside by tool diameter plus 10%:
and cut that and the pocket to suitable depths:
Next we need geometry and toolpaths for cutting the dovetail slots for the bottom:
We draw a circle the same diameter as the geometry for the dovetail slots:
and duplicate it and align a copy at each end of a slot:
and draw a line from center-to-center:
duplicate it in place, and select it and the outline and use Mirror Horizontal to move the copy to the other side:
Check that the lines are far enough from the box outline by dragging the drawing of the dovetail tool over:
Then assign a pair of toolpaths, one to clear the slots w/ a suitable square endmill, the other to cut the dovetails with the dovetail cutter:
Next duplicate the circles and the lines drawn for the dovetail tool and adapt them to cut out the dovetails for the top:
Offset the outline of the outline of the top:
and then select it and the pockets:
and use the Trim Vectors tool to create optimal geometry for removing the bulk of the material for the top:
arriving at:
OK
OK
which may then be joined together:
Yes
Additionally all of the circles for the entry/exit points for the Dovetail tool should be instantiated at that tool’s diameter:
and unioned with the pocket toolpaths so that as much material as is possible will be removed before the Dovetail tool cuts:
It is then possible to rotate the Dovetail slots for the bottom and move them into register with the pockets for the bottom:
and to repeat the process for the top:
at which point the file may be saved and the duplicated to make separate files w/ appropriate thickness for top/bottom.
Thinking on this overnight, a better thought than using the No-offset contour w/ the open geometry would be to just put in circles at the origin:
and then use those with a Keyhole toolpath with the appropriate settings:
It is just necessary to work out the requisite length (and angle).
I think I would start with a straight end mill no wider than the narrow end of the dovetail bit to remove as much material as possible in less than full depth passes.
Yes, that is mentioned above (but apparently not made very clear).
