Full blind box joints in Carbide Create

[WillAdams (William Adams (Carbide 3D))]

Lastly we draw in the V endmills cutting the corners in the profile view:

6 passes will be necessary — one easy way to draw this is to stack up 6 copies of one-half of the endmill:

and scale the width of it to the stock thickness:

The bottoms of each may then be measured to determine the offset from the edge/top of stock, but the first thing which should happen is drawing in rectangles which are inset by stock thickness from the face rectangles and assigning a no-offset Contour toolpath to them at the top of the stock (well, 0.001mm below the top of stock — it’s not possible to assign a depth of zero to a toolpath):

This covers the case of the stock being thicker than expected.

The next two V contour toolpaths continue this, working down by first one quarter the distance, then to half the depth of the endmill diameter plus 10%:

For each successive layer, draw a rectangle of a size to match the desired depth/offset:

Node edit it to make it into an open polyline:

Then duplicate it in place, select the face rectangle and rotate the duplicate into position, repeating this to get each corner:

assign a toolpath to an appropriate depth and then duplicate and position for each face and repeat for each other depth/face:

[WillAdams (William Adams (Carbide 3D))]

Which previews as:

Need to check that everything connects as it should — hopefully test cut tomorrow, then once I have a working file, will upload.

[WillAdams (William Adams (Carbide 3D))]

Cutting went well:

Cube_45mm_Center_Bottom.c2d (308 KB)

[WillAdams (William Adams (Carbide 3D))]

And a very quick test-fit went well:

[WillAdams (William Adams (Carbide 3D))]

Been working on this a bit more, and have automated it using OpenSCAD Graph Editor and the library I’ve been using, gcodepreview:

[WillAdams (William Adams (Carbide 3D))]

Revisiting this after completing:

Tool paths for different sized dovetail bits

I tried this with first with a pocket cut using 1/4 end mill leaving a 1/2 inch wide pocket,. Then with the dovetail bit mounted set to finished depth tried to route a pocket set 1/4 wider, but at the same depth EMPTY TOOL PATH was the result. The dovetail bit is 14 degree x approximately 7/8 wide . There aren’t any in the tool list so I thought that I could tell the machine that I was using an 1/4 in. Endmill bit

and reviewing the above as well as the various linked projects and other efforts, some thoughts/considerations:

• the new OpenPythonSCAD and the ability of gcodepreview to output open geometry in DXF works — if one opens in LibreCAD first and re-saves as SVG
• directly tracing the tool outline where appropriate is simpler to calculate since one can just use a command which includes outputting the DXF code in addition to making the cut
• where appropriate, one can always use a separate command to create arbitrary closed geometry which matches some aspect of a cut
• it is easier to block out prototypes in BlockSCAD than it is to create finished designs in OpenSCAD Graph Editor — most likely because of the difficulty of repurposing chunks of code and ensuring that slight variations in code have differences in appearance which are suitably expressive — this probably warrants further experimentation
• using 3 tools seems to be the best mix of ease-of-use and capabilities:
  • large V — note that if the library is set up to do this in one pass this will bound the maximum possible Stock Thickness — setting it to always make two passes seems expedient
  • small V — this needs to be a reasonable dimension, sufficiently smaller than the Stock Thickness that it will allow a reasonable size of Box Joint to be cut
  • small square — if doing this in a graphical tool it may be helpful to use a smaller diameter than the Small V (3mm vs. 3.175mm is one dimension pair which I considered and sourced tooling for), but if one is directly modeling toolpaths, having a direct correspondence is more straight-forward

Starting by roughing out the design in BlockSCAD we have a pretty standard set of parameters to begin:

stockXwidth = 0;
stockYheight = 0;
stockZthickness = 0;
Joint_Width = 0;
Number_of_Joints = 0;
Large_V_Diameter = 0;
Small_V_Diameter = 0;
Small_Square_Diameter = 0;
Joint_X_Position = 0;
Joint_Y_Position = 0;
Joint_Orientation = 0;
Joint_Side = 0;

Note that it will be possible to position a joint both in terms of XY and in orientation and to specify which side of a joint is to be modeled/cut, allowing arbitrary part orientation.

[WillAdams (William Adams (Carbide 3D))]

In setting up the initial values, the first question which arises is the number of pins — rather than doing the math, it is simple to just draw things up in Carbide Create:

draw a pair of grooves which will define the begin/end for a pin:

Scale them by 10% along the axis of the joint:

Done

then drawn in blocks for the miters:

position relative to one:

Then use Linear Array to make as many duplicates as are needed to (more than) fill the interstice:

delete the extra:

Then align:

and count:

then we fill in the other values:

and create a module:

and draw in the stock and set up an initial cut:

which has a simple analogue in Carbide Create:

[WillAdams (William Adams (Carbide 3D))]

The drawn-in rectangles indicate the material to be removed to define the pins of the joint:

and the cut through this is easily envisioned and drawn up by placing circles at each relevant point:

(using the Align tool to guide placement)

at which point the centers may be connected with a polyline:

which may then be duplicated

mirrored

and aligned:

then an array made:

and delete the extra piece:

and assign a No Offset Contour Toolpath:

[WillAdams (William Adams (Carbide 3D))]

First, do the math to get the beginning point:

at which point one can just do a loop:

with a bit of a trick to do the other side:

[WillAdams (William Adams (Carbide 3D))]

Then make the cuts at the ends:

as discussed above, the cutting depth of the Large V diameter tool is a limiting factor, so it will be necessary to add additional cuts offset by some proportion of the Stock Thickness — which should be included at the appropriate if statements.

[WillAdams (William Adams (Carbide 3D))]

which just leaves the matter of working out how to get the pins to fit into the cut recesses which are necessarily rounded — one option would be to use a roundover tool working up the geometry of rounding each pin, but it is more expedient to make a V cut to the depth of the small tool and cut with a square tool in-between:

[WillAdams (William Adams (Carbide 3D))]

And to make a second version of all the code which supports the horizontal orientation…

[WillAdams (William Adams (Carbide 3D))]

Duplicating and rearranging things we get: