Let's make a coaster

Software Carbide Create
1

The prototypical first job for a Shapeoko is to cut a coaster — here we do this using Carbide Create, trying to make the job as simple as possible, but adding a bit of interest with an inlay, and increasing the utility of the object by rounding off the corners.

Before any real setup it will be best to go into Job Setup and Clear the drawing, and set the measurement units — please use mm (metric) for this tutorial. Note that the feeds and speeds in the Carbide 3D charts are given in Imperial inches, for metric please see:

First, Job Setup — we will use a just over 3/4" (19.3mm) thick piece of poplar for this, and a 1mm thick piece of walnut (naturally, you may use any suitable materials, in any reasonable thickness — just measure them and substitute your own measurements throughout). We’ll do this in one file, so we’ll manually need to manage the walnut inlay thickness later. We want the piece to be 78mmx78mm (the actual stock could be larger, but this is what we want to manage/cut), so we will input:

  • Stock Size
  • Width (X): 78.000 mm
  • Height (Y): 78.000 mm
  • Stock Thickness
  • (Z): 19.000 mm (please adjust this value to match the thickness of your stock)
  • Top — we will be registering off the top of the material as zero to begin the cut
  • Toolpath Zero
  • Lower left — we will leave this at the default, so when zeroing, will need to position the stock so that from the point we set for zero there will be 78mm of material farther into the machine, and to the right, and 19mm (the stock thickness) of material beneath the zero point

Set Material and Machine and retract height to match your setup and workholding situation.

  • Units
  • mm — please use metric for this tutorial
  • Document Background
  • please click on the Edit button

I also set the background grid to be 6.5mm, since I prefer things neat, tidy, and integral and it will be necessary to make the rounded corners as described below. Please note that since this tutorial has been done, rounding corners as been added as a fundamental feature in Carbide Create, making this sort of thing much simpler (the tutorial below may still be useful for covering Boolean operations and snapping / aligning parts).

click Ok here

Then, when back to Job Setup, scroll down if necessary and click OK

1 Like
2

If necessary, click on the Design tab at the upper left.

Begin the design by making the inlay — a circle in the center for this tutorial (you could try again with other shapes — please see the Library of Design Elements) — the circle should be centered at 39.00 X, and 39.00 Y with a radius of 26.00 mm — select the circle tool

carbidecreate_screen_circle_arrow
carbidecreate_screen_circle_arrow.png1919×1080 62.6 KB

click at the center,

carbidecreate_screen_center_arrow
carbidecreate_screen_center_arrow.png1919×1080 50.3 KB

then move to the next to the last row and click again:

You may now assign a toolpath to this and go ahead and cut it out:

  • Toolpath | Contour
  • Tool | Edit to select an appropriate endmill (this should be a flat-bottomed one, 1/8" or 1/4")
  • Set Speeds Automatically
  • Cutting Depth 1.00mm — this should be the same thickness as the material which is intended for the inlay
  • Offset Direction | Outside / Right
  • Name | Inlay cutout — get in the habit of naming all toolpaths, and for more complex jobs, work up a suitable scheme for this

1 Like
3

OK

Show Simulation

Hide Simulation

Save G-code — put this somewhere convenient, clamp the stock, open Carbide Motion, connect to the machine, jog to the desired origin (should be bottom left of the 78 x 78mm square – not that you can use a larger stock, the 78x78mm size represents the minimum), set zero, send the file

1 Like
4

right-click on the toolpath and Disable it:

Arguably it would be better to go ahead and delete it — disabled toolpaths seem to confuse the software.

1 Like
5

Now we want a pair of rounded rectangles — these will be created from two stacked rectangles and four circles drawn in at the corners (EDIT: since this tutorial was created before Carbide Create had an easy facility for this — the instructions for doing this using Boolean operations are left here for didactic reasons — the reader may instead use the automatic feature for expediency).

First draw the rectangles:

Then draw four circles at the corners, with a radius of 6.5mm:

Do a drag-select to select the two rectangles and a circle:

then do a Boolean Union:

repeat with the resultant shape for the other corners:

Then duplicate this path (Control c), and set it to be centered at 39 X, 39 Y, and then scale it to 78 mm:

1 Like
6

With all the paths created, it’s a matter of creating toolpaths. We start from the top and work our way down:

  • pocket cut out so as to define a ridge around the coaster (middle path)
  • pocket cut from the base of that for the previously cut inlay piece
  • profile cut to define the piece and cut it out
1 Like
7

Click on the middle path:

Toolpath | Create Toolpath | Contour

set things appropriately, OK

Select the circle and assign a suitably deep pocket to it:

Lastly, select the outermost path and assign it an outer profile cut:

Toolpath | Cutting Depth: check Use stock bottom (we want to cut all the way through) | Offset Direction: Outside / Right | Name: coaster outer profile | OK

Show Simulation

make sure everything is okay, then save as before.

Once everything is cut out, glue the inlay in place with a water resistant glue (I like Titebond III), and finish with a water resistant finish such as a spray polyurethane — optionally, one might make the inlay of cork, or some similar material, in which case I would suggest finishing the wood, then gluing the inlay using contact cement or some other adhesive which would be compatible with the finish used.

1 Like
8

I would be grateful if anyone who had some time to spare would try out the above, and let me know (preferably via a PM) of any difficulties or issues in completing the above tutorial.

2 Likes
9

Hey Will,

I am new to carbide and cnc in general. My Shapeopko will arrive in 4 days. I have been trying to find a simple way to do inlays in carbide create. I have faith that the above will work, because the shape is round.

Let’s picture a star. I thought, well I can just cut a pocket, then on the same shape, cut an outside path. But I think the pocket will have a slight radius and the outside cut will end up with sharp corners on the tips of the stars. Am I thinking about this correctly?

I then looked at your other post here:Inlays using Carbide Create (and other software)

but I am intimidated a bit by the designing/math of it, and a friend of mine convinced me to buy the 91 degree bit instead of 90, so I’m not sure it would still work.

Is the only option to design rounded tip vectors?

Thanks in advance, happy to try this out when I get up and running.

Freddy

10

Pretty much. 90 vice 91 degrees ought not matter — too small a difference.

c.f., Inlay Work (Woodworking) - #2 by WillAdams and