Tiling Large Jobs, Flipping

I’ve got a few things queue’d up that are larger than my S3 can cope with. I have vcarve, so tiling is an option. I’ve not done much with it, but watched and read many a tutorial, all of which revolve around the “slide the stock through” method. As my CNC is in a corner, I can’t well slide anything through it. I’ll need to rotate a piece end-for-end.

As far as I’m aware there is no “native” functionality in vCarve to take care of this, have any of you ever done “manual” tiling where an end-for-end (180 degree) rotation of the workpiece was needed to complete the other half? I’m trying to work through mentally (and in CAD) how I would design the tiles for this… Cut the vectors in half, then flip one 180 degrees?

Any thoughts welcome…

1 Like

I have a similar set-up and did just what you suggested in your last sentence. I had to also turn the work piece around and carefully reset the work origins to match the rotated workpiece and panel to cut. It wasn’t too difficult and worked just fine.

I’ve done it on a nomad (it has a 3 sided case). You have to be very careful about getting the x/y zero set. The way -I- did it with meshcam:

  1. Create a “machine in” region around the first chunk to machine.
  2. place a hole towards the edge, that you can overlap a little with when you turn the whole thing around.
  3. Put the x/y zero in the middle of the hole.
  4. Generate a toolpath for the first region.
  5. Rotate the part 180 degrees against the machining axis.
  6. Clear all the regions. Create a new one that overlaps the hole, and put he zero into the middle of the hole. Your fore/aft axis should now be pointed in the opposite direction from the first tile.
  7. Generate your new toolpath.

You now have a first and second toolpath.
Place your material. This is trickier than it seems. To keep this easy, you need a reference on the material you can align with the x/y axis. If you can’t align the material when you rotate it 180 degrees, you will end up with the two tiles “skewed” against each other. That means you need your material to have square (90 degree) corners, with straight edges between them. I use a couple pins in the wasteboard to align against. All the pinholes in my board are aligned on the x and y axis, so I just pick some convienient ones, and but the material up against them firmly. Clamp your material. Set your zero carefully on where the registration hole will be. Cut the first toolpath. Turn the material around, again, firmly against a set of pins aligned with the axis, and clamp it. Put a dowel pin (metal) into the collet that is the same size as the registration hole. Carefully set your zero so that the dowel easily runs in and out of the registration hole. Take your time. Put the tool back in, run your second toolpath.

Getting the zero set the second time is really fussy.

I -strongly- recommend you do this a couple times with scrap material before committing something you can’t afford to throw away.


@mikep Thanks a ton for this, makes me feel better knowing I was at least on the right track.

I’m going to give this a whirl in the morning on a tiny test piece to validate the procedure. I’m going to use a pair of milled indexing holes through the stock across it’s width, into the waste board. I’ll then pin it there, mill job 1, flip it around using those holes to re-index, then run job 2 without any rezero. I’m using the center of one of these holes as my work origin and kept copies of all my vectors to keep the shapes spacing relative to the indexing holes the same on both jobs… we’ll see how it goes!

Thanks again for the input!

Following up after some testing today:

Big success! I used the following (rough) method:

  1. Created my vectors
  2. Added two 1/4" index holes along the X axis on either side of my work, outside the finished area
  3. Duplicated my vectors WITH the index holes, split them down the middle and rotated one of them 180*
  4. Exported three toolspaths: One for the index holes, one with Half1 on the X axis, one with Half2 on the X
  5. Mill the index holes
  6. Mill Half1
  7. Flip the part end for end, using the holes to line it up
  8. Mill Half2

Went very well, twice, in small scale. I’m going to man up and do a bigger project… maybe tomorrow.
If there is interest, maybe I’ll do a quick video on setting it all up too.


Having a video of this process would probably help out a fair number of people. I know when I did it I would have really appreciated a way to watch someone do it first!

I started working out an example here tonight and no kidding, Carbide Create can’t correctly rotate or flip a group of vectors :sob: Selecting a couple vectors and doing a rotate or flip results in skew across both axis that gets worse the more times the flip is applied. Guess I’ll do the example in vCarve :frowning:

I rotated the vectors outside of CC (in Illustrator) and just used CC to assign the toolpaths.

1 Like

Here’s how I did it. I do my drawings/designs in Illustrator but what I did should work similarly using Inkscape, Corel or other vector drawing program. I first prepared the workpiece and brad nailed two wood strips to the wasteboard absolutely square to the machine so that the workpiece fit snugly between.

Knowing the exact dimensions (length and width) of the workpiece I first drew a rectangle box in the drawing program to match those. Then I place the design/letters (outlined) inside the box positioning and sizing them as I want. Then place a line across the box and design and divide it all into two pieces ending up with the design and the box cut into two separate groups of objects. I rotated one of those 180 degrees then made each section into it’s own svg file.

When I open the first file in CC it comes in with the divided rectangle box (and it’s contents) aligned with the bottom left, which is where the work zero is set. I select the objects within the box (but not the box) to assign toolpaths as required. I do this for each of svg files.

Then I secure the workpiece in the machine between the holding strips and carefully mark or install a wood stop where the end of the workpiece is (which is also job zero on the forward left side) Then I jog the machine to that forward left corner, set the workpiece zeros and run that first .nc file.

After the first file is done I turn the workpiece around and put it between the holding strips and secure it with it’s end lined up with the mark or the stop piece. I rapid position back to the workpiece zero set for the first section and run the second .nc file.

I’ve only done it twice but both times worked just fine.

1 Like