In this tutorial, I will show you how you can make a woodcut relief print using a CNC machine. I use F-engrave (free software) to make the Gcode and UGS (Universal Gcode Sender) to run the code on my Shapeoko 3. I also use Adobe Illustrator to make the DXF file, but Inkscape is a good free alternative.
(article continue below the video)
First Things First
So what is a Woodcut Relief Print? It’s simply a very old technique for making prints using a piece of carved wood and ink.
Woodcut is a relief printing technique in printmaking. An artist carves an image into the surface of a block of wood—typically with gouges—leaving the printing parts level with the surface while removing the non-printing parts. Areas that the artist cuts away carry no ink, while characters or images at surface level carry the ink to produce the print. The block is cut along the wood grain (unlike wood engraving, where the block is cut in the end-grain). The surface is covered with ink by rolling over the surface with an ink-covered roller (brayer), leaving ink upon the flat surface but not in the non-printing areas.
Step 1 – What to print?
As you can see from the example above (Four Horsemen of the Apocalypse by Albrecht Dürer) you can make very complex artwork, but as with all great art that would require some serious artistic skills. Albrecht Dürer made that print over 500 years ago and he (obviously) did not have a CNC machine. It was all carved by hand. The funny thing is that even with modern technology 500 years later it would require pretty good CNC machining skills to make something like that, and then I’m only talking about the carving process. The artwork require a true master. However, I am going to make something a little less complex, but still very cool.
When selecting what artwork to carve for your woodcut print there are some things you need to consider to avoid problems. Here are some tips:
- Begin with a simple design or shape to learn how things work
- Avoid too many details in the beginning
- Making a logo or even a simple text is a great first project
Step 2 – Preparing The Files
Open your artwork vector file in Illustrator or Incscape and make sure you have a border around your artwork as in fig.1 below. To make the relief we need to cut away the white areas. Export your file as DFX.
Import file to F-engrave
The next step is to open your DXF file in F-engrave and set the parameters for your carving. In fig. 2 below you can see my settings.
- At the bottom left make sure f-engrave is set to V-engrave.
- Set the size you want. I set mine to 200×200 mm but as you can see it says 208×208 mm at the bottom of the page. This is because I make a frame around the artwork (4 mm on each side). More on this later.
- Where you want your spindle/router to start. I select bottom left.
- This is where you set the properties of your machine (how fast the machine is goint to cut etc. This depends on your wood type, image details and router bit. Hardwood with a smooth surface works best (I think). Try to use a sharp router bit and don’t go too fast (especially if your artwork contains many small details).
- Note! Check “Mirror image” if you haven’t done this in illustrator or inkscape already.
Next you need to go to Settings–>V-carve settings from the top menu. Here I go through all the settings we need to set. I’ll start at the top.
Set cutter type to V-Bit and set the parameters below to match your router bit. Note that the V-bit Angle must be set to 90 degree if you are using a bit that cuts 45 degree v-grooves (see router bit illustration next to the check boxes).
The depth limit depends on your material thickness and router bit (make sure you use a minus before the number). The depth also affect the work load and can cause bad quality if the load is too high. I set the cut depth limit to 4 mm, which should be no problem with the bit I use and a fairly slow feed rate.
I don’t think I have ever adjusted the sub-step length, I just used the defaults. You can learn more about this in the F-engrave manual if you want.
Next you ned to check “Flip Normals” and “Add Box”. This will make sure you cut outside of your closed paths (the white area in the vector file). I set “Box Gap” to 4 mm which is the width of the border around the image. Skip the “Prismatic” and “Multipass Cutting” fields.
Set the “Cleanup Operations” as shown in fig. 3 (“Cleanup Cut Diameter” is the size of your cleanup bit, adjust if needed). Do not hit the “Calculate Cleanup” button yet. Tap the “Calculate V-Carve” button at the bottom of the window and the program should now generate the tool paths for your main cut (this may take a couple of minutes) like fig. 4 below.
First file ready
Now your main file should be ready to save. We need two more files so make sure you include the number 1 in your filename when you save it so you know that this is the first file to run. Now, let’s take a look at the toolpaths in fig. 5. As you can see there is a thick black area with thin lines inside around the artwork. The black area is where the router bit goes and the white lines represents the center of the bit.
Now we need to make two more Gcode files for our cleanup process. The first cleanup is done using the same v-bit as in the main cut. On the second cleanup cut we must change the bit. Let’s take a look at fig. 5 below. Open the V-Carve settings from the top menu again and hit the “Calculate Cleanup” button. Now you might notice some yellow lines in the toolpath, this is the cleanup path done with the v-bit. The red area is the 4 mm straight bit wich is our final cleanup. Save cleanup Gcode and V cleanup Gcode (remember that you must run V cleanup Gcode as the first cleanup process).
Step 3 – Carving
Carving on the CNC machine
A piece of thick, flat hardwood like cherry or walnut would probably be the best option I but for this test I used birch plywood. My piece were not perfectly flat so I lost some details and some lines were not perfect but it turned out very nice anyway.
Now that we have three Gcode files we can fire up our CNC machine and UGS (Universal Gcode Sender). Now you need to run the first file (main carving) and when it’s done run the first cleanup file (V-Bit cleanup). Remember to return the machine to zero before you run the cleanup. When the second file (first cleanup) is done you need to change to a straight bit (whith the dimmensions you set in F-engrave). You probably need to raise the height to change the bit so raise the router manually by tapping the Z-axis button (don’t touch anything else). Once you have changed the bit lower the macine manually back down to touch the work piece (do NOT use the return to zero button this time).
When you are done with all three files your woodcut printing plate is almost ready but first you might need to clean it up a little and give it a light sanding. It would also be a good idea to coat it with some laquer to avoid the ink soaking into the wood. I also sealed my plate with some wax.
Step 4 – Printing
Now that you have carved and prepeared your plate you should be ready to print. Do not use paint since it can fill up your plate and mess up the details. The best option is to use block printing ink and a brayer roller.
Roll a thin layer of ink on your plate and carefully lay your paper over. Use a spoon or clean brayer roller to add pressure.
If you have any questions or anything is unclear please leave a comment below.