For our daughter’s birthday, we noticed how much she seems to enjoy dollhouses so we decided to build one for her. She has plenty of dolls she could use with one, by she doesn’t have the house itself. We have always made her gifts (Last year was a ukulele — yea, yea, we know she’s way too young for it yet… give it time) and we really didn’t want to buy a dollhouse made out of a whole barrel’s worth of oil. Since I’m no CAD star, we looked online for good plans to use.
We came across this Etsy seller and in particular this design. For less than $15 we got the plans which can be used for either a router or a laser cutter and either 5mm or 6mm plywood. For $20-30 we got the flattest and prettiest sheet of quarter-inch plywood from home depot and had it cut in 2′ x 4’ sections to fit in my car and my machine.
At the bottom of this article I have a bullet checklist with a quick reference of all my tips for this project.
My machine is the Xcarve which has the cutting area of about 32”x 31” and the dollhouse plans are HUGE in comparison, so I have to make separate panels for each piece and can’t cut all in one go. I found that the Xcarve is nowhere as good as a shopbot in terms of precision and rigidity so I ended up doing a lot of small test cuts rather than large cuts anyway.
The first hurdle I had was that while the plans I bought came with 4 different file formats, (Abode Illustrator, AutoCAD dxf, CorelDraw, and SVG) When I imported the SVG into Easel, it garbled some parts. Some parts were solid shapes and I could not simply select to cut the outline of the shape. The problem was that Easel likes to have “closed” so the lines used for decoration (like the shingles) wouldn’t cut.
I’ve only cut a couple of projects with Easel which I find much simpler to use than other CAM/Gcode-sending software, but haven’t had tons of luck with external CAM. This led me to hunt for a better option. I had seen online that MakerCAM could do open vectors, but I found it tedious.
I ended up using Carbide Create (originally for the Shapeoko 3) which is adequate for the most part.
The workflow is as follows:
Open SVG in Carbide Create –> build toolpaths –> export Gcode file –> import gcode into Easel –>Send to machine.
If you use another machine or controller software, just replace the last 2 steps with your software.
I found the default feeds and speeds in Easel were way too conservative. For each toolpath, I tested on the smallest part of the dollhouse, the windows; which I needed a bunch of anyway. Playing with the SVG showed that the dollhouse design had dogbones in the interior corners (as it should) and those were approximately 1/8” in diameter which gave me the size endmill I needed to use.
You can check out this official series of videos for basics in Carbide Create.
The order you cut the line in the design actually matters. You want to cut all decorative engraving first, then interior cuts, and finally the outlines. Select all the design elements you want engraved (if your design has any) and create a toolpath for them. In my case all the open shapes in my SVG file (which Carbide Crete shows as pink) are what I want to engrave. Holding Ctrl, I click each line I want, then click the “Contour” button near the top left of the screen. This opens the “toolpaths” section which you can always get back to by clicking the green “toolpaths” button at the top of the screen. I select a 1/8” (0.125”) flat endmill for my tool. In my case, I created my own tool to play around with it. Then to override the incredibly conservative default feed rates, uncheck “Set speeds and feed automatically” so you can type in the boxes below.
Since I’m using a 0.125” endmill, the typical stepover and stepdown rule of thumb is these should be no more than 0.5*endmill width which in my case is 0.056” each for the maximum speed. I am using a 4-flute 1/8” bit at 10,000RPM, so I should be able to fly through these cuts. The default feedrate is 12.5 inches per minute (IPM). Easel’s default for a single-flute 1/8” is 40IPM. Since my bit as 4 times as many cutting edges, it’s able to remove material about 4 times as fast as a single flute but I set the feed rate to 40IPM. The 10,000RPM is too fast for what I’m trying to do, but that’s as slow as my router will go.
The next step is to set up the type of cut, max depth, and if you want to add tabs. Since these are superficial cuts, I want to just have the center of my endmill follow the path of the line so I use “no offset”. Since I’m starting my bit at the top of the material, I leave “Startdepth” to 0.000in. I only want an engraving so I use 0.06 inches depth. My material’s thickness is 0.21in so this should be a nice relief. It is also deep enough to not have issues with my unlevel machine. As long as I get the impression of the lines it is OK if they aren’t all the exact same depth, though this is something I should fix in the future. There is no need for tabs on this cutting path so I ignored that option for now.
At this point you can try to see the simulation of the cut, but as of the version I am using the simulation is not very accurate as shown in the full simulation of the part below. Several lines are completely missing (which actually did cut just fine) and the engraved contours have random jagged areas (which don’t appear in the real cut). I recommend avoiding the simulation in this software at this time.
I saved the engraved cuts as “siding” which you can see highlighted in red below.
The next set of cuts are all the interior cuts such as the doorway and the slots. Holding Ctrl, click each item you want, then set up a cut for the interior (the default selection). Don’t forget to change the stepover and feedrate, otherwise it’ll take you many times longer to finish the cut. For the larger areas (not the slots) I added tabs. Tabs on these pieces are areas that don’t cut completely through so the interior part doesn’t wobble around and break stuff when it is cut out. To add tabs, in the toolpath simply click “Edit tabs” and then click on your shape where you want tabs. Tabs appear on your drawing as a little box with an ‘X’ in it. I recommend only having a few tabs (the fewer you have to clean up later) and placing them strategically. For instance, due to the unlevel-ness of my machine, sometimes my tabs are only as thick as the bottom facing of the plywood which is sometimes not strong enough to function as expected. This also depended on the grain direction and direction of the cut. For instance, the tab on the left side of the doorway broke because the grain of the facing ply was vertical and so was the direction of the cut. I also tweaked the tab size to make it hold better and easier to cut when the cut finishes. 
I saved this as “InnerCuts” which is shown in red below:
Finally I made the toolpaths for the exterior cuts. I used all the same depth and stepover settings as with the inner cuts. I added some tabs and this toolpath as “outside cuts.” I honestly changed up the cutting speed to up to about 55in/minute and didn’t really see any detrimental results. You can play with these settings to see what works best for your job and set up.
Once all the toolpaths are set up they need to be exported as g-code. While you can export them all as one file, and they would execute top to bottom, I strongly discourage this. Export each one separately because if something happens and you need to recut (maybe you didn’t go deep enough on the first try, etc.) you can always go back to 0,0,0 on your machine and make tweaks to the starting position as needed and try again.
I imported the gcode files into Easel.com to send to my xcarve. You can import gcode by going to File—> Import gcode.
I loaded the three files in the same order as I had created them. Engrave, then interior cuts, then exterior cuts. Each one is automatically loaded into its own “workpiece” as shown at the bottom of the screen. In this example, I actually only did the bottom wall because I forgot to save screenshots from the workflow above. Just note that whatever you set up in your toolpath should be shown in Easel.
Midway through the project, Inventables added the easily-accessible Jog feature to Easel which I found to be incredibly helpful. Since then, there are lots of new features that have been added.
I loaded the wood onto my machine. I was using 2’ft x 4ft sheets of 1/4″in Sande ply. We actually bought two 4ft. by 8ft sheets at the orange big box hardware shop and had them cut it to the smaller size for us to fit in the car.
The xcarve can’t cut the full 4ft length, but I loaded it into the machine without shortening it. This is because once I cut a full-size panel, I then flipped the plywood around and cut another piece on the previously unreachable area.
To mount the plywood, I use the same method I used for manually planning guitar blanks in the past with great success. After laying down the plywood on the machine with the bowed par facing the table (bowed edges flexing upward)and getting it relatively straight and in line with the X and Y motion of the router I laid down a strip of 2” masking tape on my spoilboard halfway under the wood running the length of the board. A tip here is don’t align to your rails or you’ll have a bad time.
After realigning the plywood, I go back and glue the edge of the board to the tape using a high-temp hot glue. To flatten out and bowing the in wood I use my free hand to apply pressure an hold until the glue is hardened, or you can set some clean heady books on it. You don’t really want the glue under the wood, just along the edges. Since we laid the bowed part of the wood into the table, that’ll make it easier to not have a ”bubble” in the middle of our wood that would mess up any cut depth there.
Throw your 1/8” downcut endmill into the collet and you’re about ready to cut. You want to use a downcut endmill because it if there is any bow or warping to the wood, as it cuts the force of the flutes will put downward to help flatten the wood. This also leaves a much nicer finish on the top of the wood. Sadly, I didn’t find all this out until after I made all my cuts and as you can see below, had to manually use a razor blade on all edges to clean them up.
Once the glue is set, I turn on the machine and click “Carve” in Easel. I can then jog the router to the bottom left corner just to the interior of the wood by about the size of my bit on each axis. This will give me a margin of error incase I didn’t align my tape very well.
After zeroing X, Y, and Z, I jog the z down slowly until the bit presses about 0.1” into the wood. This will help me realign if I need to hit the E-stop and lose my home coordinates.
I quickly turn the router on and off to make a small indention here. If something catastrophic happens and I hit the E-stop or lose power and my machine forgets its location, I can manually adjust my X and Y locations until the bit fits snuggly into this divot and I know I’m pretty close to my original zeros. I zero the X and Y axes at this spot. Lift the bit and move over the wood just next to this divot (I usually move X to the right 1”) and bring the Z axis to touch the top of the wood. I actually put a little pressure on the wood by a couple 0.001” movements.
Part of the workflow in Easel allows you to zero the Z axis by itself after you confirm your location and material thickness. I zero the Z axis at this point. Then in the Job menu, I bring the bit up a touch and move back to X=0 (move X back to the left 1”). Then you are ready to cut.
It’s loud, so wear ear protection. Also wear a dustmask with the appropriate particulate filters. I have a dust boot on my machine, so I set that up. The vacuums I have for my dust boot consist of a household vacuum we’ve had for like 15years that recently lost a wheel and a tiny shop vac. Neither of these were designed to run for hours on end in 90+ degree weather (in the garage with the door open in the middle of NC summer). They both overheat during the cuts so I cycle them out as often as I can. I also run my air filter the whole time and for a few house after I am finished. You might think that with the door of the garage opened you wouldn’t need this but you’d be wrong.
While cutting, if something isn’t right, it is always best to hit the Stop button unless there’s a serious emergency (like someone getting hurt). If you hit the normal stop button (wither in Easel or on the Xcontroller) the Xcarve will finish its current cut, raise the bit to the safe height and bring it back to X0,Y0, Z(safe Height). This way, you can make simple modifications to either the code and try again without losing your position. If you hit the E-stop button, the machine completely cuts off and disconnects from the computer. This will lose your current position. You’ll have to try tot manually set up your X, Y, Z which is never quite correct. That’s why we made that divot in the beginning though. Just in case you hit E-stop you can jog the bit back into that divot, raise the bit, move over and set the Z height again just as before and you’ll be kinda close.
Once all 3 cuts are finished, your part is still stuck in the workpiece because of the tabs. The easiest way to remove the tabs is to use a chisel. Place the flat side of the chisel against the part you’d like to keep and give it a stern whack with a mallet or hammer. This should break the tab and leave you with a relatively clean edge.
To remove your stock material from the table, simply pull upward near the end of one edge and the hot glue should peel off the tape. You can reuse this tape a few times before having to reposition it.
Once I had cut all the dollhouse parts, I cleaned up the edges with a box cutter and razor blades and sanded everything with 220 grit sand paper on my orbital sander to flatten it a bit. The 1/4” ply is slightly thicker than the metric 5mm of the design do for the tabs to fie correctly into the slots, I had to make sure to sand these a bit more. It’s ok if they fit a little loose too because when you add shellac it thickens the piece, then you can put on the twist-knobs to tighten the tabs to the faces of the part with the slot. This really is a genius design and works well if you sand it enough.
After the initial fit, I went back and had to sharpen the interior angles of all the tabs so they’d fit flush with the slots. Without this the design would never work.
I used my box cutter and some tiny files for this. You don’t want any overhangs because when you seal it in the next step, anything that is a soft burr of wood becomes a tiny razor blade or needle when the sealant dries on it.
Take everything outside and shellac it because Sande Ply smells horrible! I think it is formaldehyde in the glue. I sat all the pieces out in the sun for a couple of days (each side getting 1 full day of sun) in the 90+ degree heat which drove off the majority of the stank. I needed to seal it though to prevent exposing my kid to VOCs. Shellac is a natural ingredient made from bug poop dissolved in ethyl alcohol. It is FDA approved (used to coat pills for decades) and often used for baby cribs. Seemed like a great option. I had bought a half-pint of shellac and did it by hand which took forever and didn’t look great. I recommend you buy spray cans of it for fast even coats. Three or more light coats work best for sealing. Make sure to sand with 200 grit paper between each sanding and let it dry for a couple hours between coats. The result slightly darkens the wood, smooths the surface finish, and most importantly, completely seals all the pores of the wood so no chemicals will get in or out of it.
We had to sand the tabs a bit more before it fit back together, and not all the toggles cinched without breaking the tabs. No big deal, that’s why Ii have glue.
This project took quite a while to complete, mainly because of the finishing steps. It took a full 3 days of figuring out my workflow and cutting on the machine (I messed up a few times too in the learning process of course), another couple of weeks for clean up and sealing as I only worked on it on the weekends.
The final result: My daughter absolutely love it! She immediately began playing with it as soon as I brought it in the house. It isn’t the most ornate, or even well-built but I’m proud of it.
Ok, so here’s the cheatsheet for this project:
-
Get plans for the design. Either make it yourself (which could easily be several posts in itself) or buy them.
-
Carbide Create is a great offline tool for generating toolpaths.
-
Make sure to change the step over and depth EVERY TIME you create a toolpath unless you are immortal and time is meaningless to you.
-
Make sure to check the the start depth and ending depth before exporting the gcode
-
Change tabs to make sense. I did 0.3” thick and 0.118 tall since my stock material bowed a bit and I was using a 1/4” chisel.
-
Export each cut separately
-
-
Import gcode into Easel in this order: Engrave –> inside –> outside cuts.
-
Lay down wood on work area with the bowed part down (edged bending upward) and align 2” masking tape just under the edges
-
Use high temp hot glue to secure edges of wood to tape using weight to keep it flat if needed
-
Use a downcut endmill for best results and to help prevent the wood pulling upward in the flutes.
-
Move router to bottom left corner where bit is just fully inside the edges of the wood and jog Z down a bit. Turn on the router and adjust Z until you create a divot in the wood. This will serve as your way to recapture the 0,0 of the job if E-stop or power failure.
-
Zero X and Y axes to this point.
-
Move Z up and move X—>1” and use Easel’s Carve workflow to set the height of the material (which Zeros the Z axis)
-
Move the X back over the divot
-
Carve the piece.
-
Rinse and repeat with each cut
-
When finished, use a chisel with the flat side on the part you want to keep to remove tabs.
-
Sand with an orbital sander with 200 grit to remove all the burrs and sharp edges.
-
May need to use razor blades or hand-sand to get some tight spots
-
Go ahead and make interior cuts of the tabs square for a better fitment
-
Sand tabs more than you think you should. They would fit loosely in the slots and the toggles should turn easily when you put the house together.
-
Let wood sit in hot sun for a day on each side with ventilation underneath (I have a slatted patio table) to remove the formaldehyde stank.
-
Spray with shellac (don’t brush it on unless you have to for tiny detailed spots), let dry a couple hours, sand with 200 grit.
-
Rinse and repeat until all parts are sealed well.
-
Put it together and enjoy.