V Carving Colored HDPE

I did a quick project to demonstrate some of our new products.  As soon as I saw the green on white two color HDPE I thought of the Starbucks logo.  I thought a nice, deep 60° V Carving of this would look great. The Inventables products I used on this project are:


You want to use the highest resolution image you can get.  This will give the best bitmap to vector conversion.  I searched for "starbucks logo" using Google Image Search.  You can use the "Search Tools" option to filter for larger images.  I found one that was over 2000 pixels wide.  You could search for a vector file, but I wanted to go through the more complex process of working with a bitmap for this post.  A vector file would save several steps and give the best results.

V Carve Process

Start a new project in V Carve with the size of the material you are working with.  I my case that was 12" x 12" x 0.50" thick.  On jobs like this, I like to put the X,Y origin at the center of my work in case the piece is not exactly 12" square.  I then draw from corner to corner with a pencil to mark the center and zero the machine on that mark.

Next, import the image into V Carve and adjust the size and centering.  Use the Trace Bitmap tool.  On a logo like this, I like to use the black and white setting.  Adjust the threshold slider until you get the smoothest edge.  While the logo looks like it is only two colors, the edges are usually anti-aliased to produce a smoother looking image.  See the highly zoomed image blow.  The adjustment allows you to choose what colors represent the the logo and which ones represent the background.

You can adjust the other sliders and preview the results.  Here are the settings I used.

The idea is to get smooth curves where there are curves and sharp corners only where they should be.  V Carving tries to highlight those corners by using the tip of the V bit.  If you get a few accidental sharp corners it might affect the look and increase the time it takes to cut.  The V Carve program usually does a pretty good job and beginners will usually be happy with the default results, but you might look for a few and try to smooth them out using the node editing tools.

Tool Paths

I decided to use a 60° V cutting bit to get a steeper angle on the pocket.  I wanted to limit the depth to 1/4".  I used a 1/4" diameter flat area clearance bit.  I setup the tool's depth per pass to cut in one pass.

The selection of a large area clearance tool size is based on the size of the large areas.  If you choose a large diameter, it will only fit in the largest areas and the V bit will have to make a lot of small moves to clear out the smaller areas.  A smaller clearance bit will be able to get into more areas, but it will take a longer time in the large areas.  See the image below of the V bit tool path.  As the areas get thinner than the clearance bit, you can see the work the V bit has to do.  The distance between v bit moves in this mode is adjustable, but I accepted the default of 0.01 inch for this project.


V Carve can give you a pretty good preview of the results.


I was very happy with the results.  The material cut great.  The deep depth of the cutting gives a a really rich look.


  • If you are using a spiral bit with HDPE, try to ramp it into the material.  The material is a lot less likely to climb up the bit
  • The corners come to a sharp point at the top of the work.  In the case of two color HDPE this will happen above the color change.  You might want to set Z zero as the top of the white if you have a lot of fine details.  With that said, I did not do that on this job and it looked fine.


Sorry, I can't share the files on this project because I don't want to deal with a bunch of over caffeinated lawyers.

Circuit board milling on the Shapeoko 2

I've been working on using the Shapeoko 2 to mill circuit boards and I thought I'd share my experiences with everyone since we get a lot of questions on the subject.

Short answer: it totally works and gives you nice clean lines. But make sure you nail the z-depth and feed speeds.

Ok, so you're going to need a couple of things here.

1. An X-Carve or other suitable milling machine

2. Circuit Board blanks, Inventables has them in 2x3" and 4x6" sizes, single and double-sided.

3. Good bits for circuit board milling. I recommend these.

Once you get all that assembled, design your circuit board. I used Eagle to set up a "stress test" of the machine, with progressively smaller component sizes and trace widths.

I then exported that as a .dxf, then used Adobe Illustrator to convert that to an .svg so I could import it into Makercam. If you're using a more professional CAM software, you could probably import the .dxf directly.

If you're unfamiliar with MakerCam, there's a good tutorial here and so I won't go into detail in this post.

Make sure you use a digital caliper and measure your bit size. It's going to matter a lot so get it right the first time and save yourself the headache.

I set up all the traces as an Outside Profile cut operation, with the cut depth as -0.25mm. You can experiment with your own settings, but I found that was the minimum depth necessary to have the bit penetrate the copper surface layer. You also want to do this in one clean pass, so set your stepdown to that same amount.

I also found that the speed settings for these boards are very touchy- there's a narrow window that works well and gives you clean edges, anything too far above or below that will give you ragged bits of copper sticking up. I recommend starting with around 150mm/min and adjusting as necessary for your machine.

Similarly, the spindle speed was a critical setting for getting clean edges. Using the stock Shapeoko spindle, I found that a speed setting of about 2.5 (between the two and the three on the rotary dial) worked best. To find the right setting, start your job and manually adjust the spindle speed until you see the edges come out clean. There's a certain amount of "tuning" here that you'll need to feel out.

Now that you've got your gcode generated, you need to plane your work area to make sure you get a consistent z-depth on the board you want to mill.

Use Makercam to generate a pocket cut for a rectangle slightly larger than your circuit board. You don't need to go very deep, only 1-2mm. 

This is going to make a nice little pocket to hold your circuit board on the work surface, and since the machine is planing the bottom of that pocket, you can rest assured that that surface is as parallel to the machine's movement as you're going to get.

People have different techniques for holding the circuit board down, but I recommend using a good sticky tape like Gorilla Tape to hold down at least three corners. There won't be a lot of pressure on the board while you're milling it, but you don't want it to slip around at all.

And here's what the end result looked like:

The traces maintained integrity down to the 0402 surface mount package size, and the trace width could get down to .12mm before becoming inconsistent. I checked the pads and traces with a multimeter and there was complete isolation/continuity on all the "experiments" except for the leftmost one in the image above, which is pretty impressive.

I believe you could get the tolerance even tighter with a better spindle and a tighter-tuned machine, but that's an experiment for another day.

Any questions on this, drop a comment below or hit us up on Twitter or Facebook. I'm happy to discuss in more detail.


Michael Una

Inventables at SxSW Create

Inventables will be at SxSW Create Friday March 7th through Sunday March 9th in Austin. This FREE and open-to-the-public event kicks off at 11:00 am. If you will be in Austin you can catch an Interactive or Film Shuttle to The Long Center for the Performing Arts to experience all the mind-expanding and hands-on fun.

We're going to be making a big product announcement and will have demo stations set up at the event for people to step up and make something.  We look forward to seeing you there.