Making cut files from simple engineering drawings

Here’s a quick tutorial on doing this.

Start with an engineering drawing for a file you want to recreate, we’ll use the filler strips from:

and open the PDF:

Note the thickness (0.75 inches) and width (10 inches) and depth (23 inches) and transfer it into job setup — note that width and depth will need to be transposed — and set the material and retract height:

Draw a rectangle:

Note that since Carbide Create draws from the center out it is easiest to draw one which is twice the desired size and then reduce to half the original size to get the desired size (alternately, put the origin at the center and begin drawing there). If need be, drag into position.

From the drawing note that the center of the holes are 0.5" in from the corners — draw a hole on that center at each corner using the Circle tool:

and then select it change the radius to make a hole of the desired diameter:

Redraw the hole for the chamfer/countersink:

and duplicate the twain and drag them into position at each corner:

Before going to make toolpaths note that the thickness would be tough to cut as a slot, so add geometry around the perimeter a bit more than 10% of the diameter of the endmill, a #201 will be used, so 0.275 inches:

With everything drawn up, it’s time for toolpaths.

But first a quick, optional detour into 3D modeling.

If you wish to model the countersink us the 3D tools afforded by Carbide Create’s Pro mode click on the Model tab.

Then select the rectangle for the part and model the stock:

select the four circles for the countersinks:

click on Shape and model them so as to remove them at 8 degrees so as to create the 82 degree angle specified:

Cutting the modeled countersinks is left as an exercise for the reader.

Instead, we will simply spot drill using a 90 degree endmill as a V carving — this will allow drilling the holes using a hand drill of the appropriate size once the filler strips are in place on the machine:

Go to the Toolpath pane and select the profile and added offset geometry and create a toolpath using a #201 endmill in MDF which cuts down to the desired depth (in this case 0.75 inches less the 0.1181 of tab thickness so 0.6319 inches):

Then create an outer profile cut which starts at the previous depth and cuts through the stock:

and add tabs:


Shapeoko XL filler strip 10 wide.c2d (80.9 KB)