A Different Sort of Tray, one cut to various depths

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

Here is a tutorial on cutting to various depths for various effects.

The goal is to make a simple open box out of a suitable material, using at least one of each tool path option.

Start by defining the size of the stock:

The box will be 3" x 3" x 0.75" (maybe more of a tray than box?) so draw in a rectangle of that size which is centered in the working area:

The interior pocket will be 2.5" x 2.5" x 0.5" resulting in 0.5" thick sides and an 0.25" thick bottom, so draw that in again centered on the working area:

At this point, one could select the center square and assign an 0.5" deep Pocket and the outer and assign an 0.75" Contour Outside / Right toolpath and be done, but where’s the fun in that?

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

The first effect we want is a V chamfer along the outside edge — this will be done with a V carving and will require adding two bits of geometry, and modifying the outer geometry for a reason which will become clear upon previewing.

When chamfering with a V endmill it is preferable that the tip of the endmill be positioned beyond where the vertical cut will be made for a cleaner edge — drawing things up in profile will help make things clearer:

So we want to inset the rectangle by the desired 1/16" of the 90 degree chamfer, and to the outside by a bit more:

and

resulting in:

and when we select those two paths and assign a V carving toolpath which is allowed to cut as deeply as it ought we get:

and when we zoom in on the preview of the path which will be followed we see a rounding at the corners:

which will require rounding off the outer geometry to match:

(that radius value may require a bit of adjustment)

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

Next, we cut the central pocket — we want this to fall a bit short, since we want to round the bottom with a ball-nosed endmill, but it’s initially a simple selection and assignment of an operation to cut to the appropriate depth — again, drawing up the cut in profile will help establish how deeply to cut:

Select the central geometry and assign a Pocket toolpath to a depth of 0.375":

which previews as:

Next, select the same geometry and create a Contour | Inside / Left Toolpath which starts at the bottom of the previous pocket (0.375") and cuts down deeply enough to fully define the rounding (an additional 0.125", the radius of the ball-nose, so 0.5" deep):

which profiles as:

Next we finish cutting the bottom of the pocket — first, inset the geometry by the radius of the ball-nosed endmill:

then select that geometry and assign a Toolpath which starts at the bottom of the pocket and cuts as deeply as the radius:

which previews as:

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

Next, we ornament the bottom with an incised design — first, draw up the design:

then assign an Advanced Vcarve toolpath which starts at the bottom of the pocket (0.5") and only cuts 0.0625" deep (so to a depth of 0.5625"):

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

To create some visual interest around the design, assign a texture toolpath which starts at the bottom, and doesn’t cut too deeply by selecting the hexagon and an outer geometry inside that which defines the lowest cut (0.5"):

Note that this may be a close thing depending on how long your reach is with your selected endmill, and how wide your collet nut is — it will probably be necessary to at least remove your Sweepy if using that for dust collection (or lift it up or use the transparent base if using v2.0)

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

Lastly we cut out the outer profile — while this could be done as a slotting Contour | Outside / Right Toolpath, it is best to add geometry and cut as a pocket down to at least tab depth — another consideration is leaving a roughing clearance and making a full-depth pass for the best possible finish.

First, offset to the outside by the desired roughing clearance:

Then offset again by the endmill diameter plus 10%:

Then select both and assign a Pocket Toolpath down to a depth which will leave the part fully secured:

(note that we’ve done the math to ensure that there will be an even number of passes to full depth)

Then select the actual outer profile and run a full depth cut which starts at that bottom and will cut through the part:

which previews as: