Any tips for machine both sides of a project?

Hi Everyone,

I’m not sure if this is even possible but I have a Fusion 360 project which is like a bezel that I’d like to mill out of a plastic. The problem is that it’s two sided with detail on both sides.

Is it feasible to be able to machine one side and then turn the stock over to machine the other side ? Obviously lining up 0,0,0 is going to be super hard, let alone the tool paths I’m yet to figure out.

Has anyone else done anything like this ?

I wish I could share the Fusion project files but it’s for a new commercial project I’m working on although I’d be interested to hear from anyone who could consult with us and maybe help with the tooling paths and setup.

Looking forward to getting our new X-Carve to compliment the Carvey :slight_smile:

All the best


There are a couple people that have done something like this, you should be able to find them with a quick forum search.

I’m considering doing something similar, and what I’ve got in mind:

  1. Center both parts of the object (in Easel) at 0, 0 in different projects.
  2. Zero Easel somewhere in the middle of your board. You will want it at least 1/2 project width +1" away from each side.
  3. At equal distances on the X axis (say, 0, -3 and 0, +3 for a part that is only 4" wide), use the X-Carve to cut round holes through and about 3/16" or so into the wasteboard. The holes should be the same size as a couple of steel pins.
  4. After cutting the holes, put steel pins through the workpiece and into the wasteboard.
  5. Maintaining X- and Y- zeroes, Z-zero Easel to the top of the workpiece and cut one half of the object.
  6. Flip the workpiece about the Y axis, making sure the steel pins are in the wasteboard.
  7. Maintaining X- and Y- zeroes, Z-zero Easel to the top of the workpiece and cut the other half of the object.

It sounds complicated, and it can be if you’re relatively new to this. If I ever get around to making my project, I’ll make a video showing how to do this so it’s easier to understand.

Good luck!


Alignment pins are the way to go, like everyone’s saying. I use a similar approach but I’ve set up my machine with M6 threaded inserts spaced at regular intervals and use those as alignment pin holes and hold downs simultaneously.

So when I want to do a 2 sided part, I mill 6mm diameter holes through the stock that line up with the threaded inserts, and then bolt the stock down to the wasteboard. Mill one side, then flip it over, and bolt it down again to mill the other side.

Bolting the stock down tightly, versus using hold downs or tape, helps prevent movement and warping during long milling sessions.

In Fusion, you’ll create two CAM Setups, one for each side. Just flip the coordinate system over for the second setup. And make sure your origin is in the same relative position for each side.


If it’s a part you will make more than one of, make a jig.

However, I plan on make a general jig for doing double sided cuts that will work for most things.

features planned for this jig
-The corner will have a built in corner finder for zeroing.
-the corner edge will be the bump stock for lining up the part
-built in clamping.

operation will be:

cut side one, flip vertically and cut side two.

The programing/designing would be done based around the jig template’s zero.

1 Like

Alignment pins sounds like a great idea!

I also considered creating a jig as we might do a small volume run if things work out.

This may be a little off topic but what I do for multi sided cuts is use a rotary axis aka indexer. I use Aspire and set up the work so zero is on the bottom and middle of the work area, cut one side, flip it 180% and then cut the other. I haven’t tried 3 or 4 sided yet but will in the future.

If you check out my part 1 video on the ghost coffin I go into some double sided machining

I am working on a video all about double sided machining


I just ran across a video of someone doing double-sided machining. It’s hard to explain, but the idea is pretty durn cool.

I bet someone could write an app to make a border like that to go around double-sided parts. Whaddaya think @paulkaplan, could it be done?

If the app could be made to a custom size with X and Y cuts being different enough to make it obvious to those of us with butterfingers, it could be centered at 0,0, then the top cut centered at 0,0. Cut, flip piece about X axis, then run bottom cut (centered at 0,0) on a separate project.

Hey guys,
I am part of a high school robotics time. I am the lead for our fabrication division and I am in charge of our x-carve. We have a lot of double sided parts( 1x1 and 2x1 tube) that requires carving. To cut the part, first, I install my piece and zero the bit. Then I take the limit switch bolts, on the gantry and side rails, and slide them over until they press against the limit switches. This way I have created a hard stop on my machine. Then, when I finished cutting the top, I manually move my bit away from the part, flip it, use the same installation holes, and slide my axis as far as they can go to the left and back. Works like a charm!
P.S. I use the 1000mm model with a custom wasteboard.

1 Like

The pins are called reference pins in machinist terms.
(Correct me if i’m wrong)

1 Like

I use Cut3D and it centers the object on a measured block.
Then you just flip it keeping X and Y at the 0 you started with.
Its how I did this. Showing only one side.

Flipboard Gadget discussion here

This is a good way of doing it. - Using the pin method.

It is missing some info though. The pins need to be along the center axis for this to work. In any case you should make them symmetrical around the flipping axis.

The other thing to note is the setup origin you need to set that to right side up for each side that you mill. I’m still playing with what should be really good origin points and I’m starting to suspect it’s the center of the stock in this case rather than my usual bottom left corner.


Hi John

It is not hard at all. I am working on a video about X-Carve probing and in it I show how I ensure that I know where I am on a work piece even after it is turned over.

Get some brass dowel (it could be any material but I used brass) that matches the diameter of one of your cutters. I have some 5 mm dowel and so I fitted a 5 mm cutter in my machine. My method would work just as well with 1/4" dowel and a 1/4" cutter.

Create a project that drills a series of holes in your waste board. There should be a row of holes (across the X direction) close to the front of the waste board. I would suggest that these should be about 40 mm forward of the Y value hard home position.

Also create a column of holes (along the Y direction) on the left of the waste board and again about 40 mm from the X hard home position.

The row and column of holes will be a right angles and you can put short ins made from your dowel in them.

Use some pins in the row and the column to create a fixed bottom left hand corner for the work piece for your job(s). When you do the toolpath for the opposite side of your piece then all you need to do is calculate the offsets from the other edge of the work piece.

This setup also guarantees that whenever you place a piece of material on the machine that it is in line and square to the machine.


Hi Robert,

No, it does not matter. As I said, if you know the size of the stock then when you flip it you can work out where the next set of toolpaths should be.


Hi Phil

I take your point and was really considering a simple 2 1/2 D project with rectangular stock.

There will be more X-Carve videos. My next one will be about probing - I keep waking up in the middle of the night with more ideas and so I may do more than one video. Having described my idea with the pins for stock location on the waste board I may make a video about that too.

Inventables have been very kind to me and they are now providing me with some modest sponsorship linked to any sales that come from anyone visiting their site via the links that I have placed in the video description of my X-Carve videos. I gave my views of the new X-Carve before I knew what they had planned.

I will also be using VCarve Pro for my projects as I am very happy with its ease of use and I know that a lot of X-Carve users have it. It also means that non X-Carve owners can benefit from what I am doing.

I am a one man band and, unlike many YouTubers, I respond to every question placed on my channel and acknowledge every comment made by viewers. For this reason my time on this excellent forum will be limited.


1 Like

I know this is a few years late, but I just got my 3018 CNC and I’m carving a waste board. The design requires machining both sides, and I can’t use pins, because the machine bed is aluminum (I guess I could drill holes in it, but really don’t want to). Can you “flip” a design in Easel?

No, but you can mirror elements or re-design so the flip-side will be carved right.