Trivets on a CNC

I recently built a table for my daughter. The phone call telling me she had ruined the finish by putting something hot directly on the table wasn’t good. That got me thinking about trivets. This is a great CNC project; an example of accurately cutting from two faces. This article includes step by step VCarve Pro design info, plus how to set up the trivet blanks on the CNC.

Router bits

Two router bits are required to make the trivets; a 1/4″ bit will be used to create registration holes and cut the trivet to its final shape and size, and a 1/2″ core box bit will be used to cut the slots. See Sources.

Make the Blanks

I made two styles of trivets. One is nothing more than boards glued edge to edge to create the blank. This approach is simple and fast. The other style consists of two layers of contrasting wood, in this case cherry and maple. The contrasting colors are exposed when you make the CNC cuts. Although it’s more labor intensive, this approach creates a more dynamic look.

My design uses a 13” x 13” blank to create an 11-1/2” x 11-1/2” trivet. Once you understand the technique you can scale your trivets to whatever size you need. The simple glue up is 3/4” thick. The contrasting blank is 1/2″ thick. I wouldn’t go under 1/2″ thick for these, but anything from 1/2″ to 3/4″ will work fine.

Create the simple trivet by edge gluing enough material to yield a 13” x 13” blank. After the glue is dry, plane or sand the blank flat.

To create the contrasting wood blank, start by resawing contrasting woods. It’s best to stick with hardwoods. A resawn thickness of 3/8” works fine.

Plane the resawn stock to remove the bandsaw marks and get it to uniform thickness. Yep, there are a lot of pieces laying on my planer. I made enough for four trivets. After planing, joint the edges of each piece, getting them ready for an edge-to-edge glue up.

Glue up the individual panels. Thin stock can be hard to clamp flat. Take it easy on clamp pressure. After the glue is dry, plane or sand the panels flat.

Glue the panels face to face to face to make up the final thickness of the blank. Use enough clamps to ensure you’ve completely closed the face to face joint of the glue up. Once the glue is dry, cut the blank to its final size; 13” x 13”.

Designing in VCarve Pro

Follow this recipe, step by step, to create the design and toolpaths.

Create a new file. Enter the thickness, width and length of the blank. Be very careful measuring the thickness to make certain you’re accurate. The best way to measure this is with digital calipers. (See Sources) XY 0,0 should be the center of the panel.

Use the Draw Rectangle tool to create an 11-1/2” x 11-1/2” square with a 1/2″ external radius on the corners, centered on the origin.

Use the Draw Rectangle tool again, this time to create a 1/2″x 10-1/2” rectangle with a 1/4” external radius.

Now we need to duplicate the slots. The easiest way to do this is by using Array Copy. Select the rectangle you just drew, create 6 rows and 1 column with a gap of 0 in the X direction and .5 in the Y direction. Click Copy and the slots will duplicate. Repeat the process using -.5 in the Y direction, and the rectangles will again repeat, filling the lower part of the square.

Create registration points so the trivet can be accurately cut from both faces. I used 3/8” dowels for the registration pins, but 1/4″ would also work. Use the Draw Circle tool to place a hole on each corner, 6” from the center line. Note that to get the holes in place on the bottom half you’ll use -6 in the X,Y Center Point boxes. Before cutting your project, it pays to test the registration hole size in scrap. Variations in router bit and dowel diameter can lead to the pins not fitting. I had to make my pin hole size .395” to get my pins to fit.

Toolpaths

Create the toolpath for the slots. The cuts will be made with a 1/2″ core box bit (See Sources) using the Pocket Toolpath. Divide your material thickness in two, add .095”, and use the resulting number as the Cut Depth. This creates just the right amount of overlap between the cuts from each face. Be sure to Ramp Plunge Moves.

Make the registration holes using a 1/4″ bit and the Pocket Toolpath. Set the Cut Depth to 3/8” more than your material thickness. Double check to make sure this doesn’t exceed the thickness of your spoilboard.

Cut the final shape using a 1/4″ bit and the 2D Profile Toolpath. Cut Depth should be .020” more than the thickness of your material. Cut Outside/Right, and add Ramps and Tabs. The tabs act as bridges, keeping the work secure while you’re making the profile cut.

Preview the toolpaths. This is a great way to double check your work. It won’t look like a trivet at this point, because we’re only seeing cuts from one face. Save your toolpaths.

Cut the Project

We’re ready to do the CNC work!

Mark the center of your blank, secure the blank to the spoilboard, install the 1/4″ bit, locate the router bit over the center point, and Zero the X and Y axes. You can also Zero the Z axis at this point. You’ll rezero the Z axis each time you change bits, but it’s important that you don’t change the XY zero from here out.

Run the registration hole toolpath. Use a vacuum or air compressor to remove dust from the holes, and insert the registration pins.

Swap out the 1/4″ bit for the core box bit. Rezero the Z, and run the toolpath for the slots. When the cuts are complete remove the hold downs and registration pins.

Flip the blank over and rotate it 90-degrees. Double check to make sure the slots you’ll be cutting on this pass will be perpendicular to the slots that are already complete. Put the registration pins in place and reinstall the hold downs.

Run the slot toolpath, swap the 1/4″ bit back in, and cut the exterior profile toolpath. Remove the trivet from the CNC, cut through the tabs, and sand the edges smooth.

A sanding mop (See Sources) works great for smoothing the slots. I use this sander on CNC work all the time.

Round over the edges with a 1/4″ roundover bit.

The easiest way to finish trivets is to dip them. Tung oil or Danish oil work great as a finish. Be sure to wipe off the excess, let the first coat dry, and then apply a second coat.

Enjoy your trivet! And save your table.

Sources

Whiteside 1/2” core box bit #1404
Whiteside 1/4″ upcut spiral but #RU4700
Klingspor Sanding Mop (assorted grits available)
Whiteside 1/4″ Roundover Bit
Wixey Digital Calipers

Discussion
  • (will not be published)

9 Responses to “Trivets on a CNC”
  1. Nesbitt Colin

    It was very clear instructions although I do not have all the machinery available to follow your instructions I intend to use a hand router to produce the trivet.

    Reply
  2. Rin

    What happened to the old days when we didin’t rely on a CNC machine for this kind of stuff?!?

    Reply
  3. G. Miller

    Are the different layers placed in opposite directions – so the CNC or router are cutting with the grain?

    Reply
    • Customer Service

      No, opposing the grain direction would probably lead to cracking. The grain directions of each layer are parallel.
      Thanks
      Paul-WWGOA

      Reply
  4. David

    Thank you for sharing this design. I will be making trivets for my wife. This design I will make on my router table with the Incra fence.

    Reply
  5. ryan

    What would be a recommendation for entry level CNC machine that could complete this project?

    Reply
    • Customer Service

      This is a relatively small project, so any number of CNC machines would be able to handle it. When you’re making your buying decision, consider:

      * How large will your CNC projects be? Machines have different bed sizes. Large projects require large beds. If you’ll only be working on smaller scale projects there’s no need to consume budget and floor space with a large bed machine

      * Budget. How much are you willing to spend? This answer will instantly dial in your choices.

      * Lots of CNC work, or only a little? If you envision growing into CNC and using it quite a bit, perhaps as a small business, a CNC with a spindle will serve you better than a CNC with a router. Spindles cost more up front, but last longer. Some machines offer the capability of coming with a router, but it can be upgraded to a spindle in the future.

      * Bits. Like a hand held router or router table, it’s great to be able to use ½” shank router bits in a CNC. Check if the machine you’re looking at offers both ¼ and ½ collets.

      * Visit a retailer. With the growth of CNC machines some retailers are now selling a number of brands. If there are any in your area this provides a great opportunity to “kick tires” and look at a variety of machines side by side.

      * Take a class. See if there are classes in your area, or informal CNC clubs that meet. This provides a great opportunity to dip your toe in the CNC water before making a purchase.
      George-WWGOA

      Reply
  6. Ted Lindahl

    I’m trying to set up your trivet project with VCarve Desktop and when I preview the tool path for the grooves cut with the .5 core box it shows to only be cutting the grooves on the right side of the vertical center line. Any ideas how to correct this.

    Reply
    • Customer Service

      Hi Ted. I’m sorry, but I don’t know what you mean by the right side of the vertical center line. Are you using a Pocket Toolpath for the grooves? It might be helpful if you send a jpeg of the Preview Toolpath image.
      Thanks
      Paul-WWGOA

      Reply