I am making a couple of larger signs that are 28 x 42, which on my machine I am limited to 32 x 32. I have watched a few videos on how to use the tile function, and the software / tool path is really nicely done on Vcarve Pro.
What left me still slightly confused was how to register the work piece, and then move it to get proper alignment for the next tile cut. This is what I did and it seems to have worked.
I planned to use a pair of 3/8 dia dowels to be the reference. I first set the work piece down on my table to make sure I could figure out where to put the holes that would be out of the way of the actual cut, and to make sure I wouldn't hit any of the T-Track on the waste board. In my case, I wanted to put the first hole 1 inch in and 8.5 inches up from the lower left corner. To do this, I made a rectangle 1 x 8.5 and used the anchor point in the lower left at x = 0 and y = 0.
I then put a .380 circle at the top right of the rectangle, ensuring I had a hole at x = 1 and y = 8.5.
For the upper hole which will be used for the second tile cut, my tile line was 21.5 inches high. When I move the board, the initial "21.5" tile line will be the new "baseline" or x = 0 line. So, I needed a hole 1 inch in and 8.5 inched high, from the 21.5 tile line. To do this, I simply made another 1 x 8.5 rectangle, but used the anchor point as x = 0 and y = 21.5. Then I placed another .380 hole at that corner.
I wanted to another pair on the other side, and I just followed the same procedure but changed the anchor point to lower right, and then changed the numbers when I made the two rectangles.
For the holes, the first lower pair I made at 1.25 inches deep to account for the dowel. The top pair, I made just .75 thick which is the thickness of my material. Another key point, I did both pairs of holes as the first operation before I made any cuts. I thought I needed the top pair of holes there BEFORE I move the board. Since I needed to make all the holes in one tool path, I needed to make sure I could reach the top pair. In this case, the top holes were 21.5 inches (tile line) + 8.5 inches = 30 inches so my 32 inch capacity would cover this cut. That was something I didn't think about until I was programming the tool path and realized that can be an issue.
So.... did it work? It's on the machine now, but yes. Here is the first tile cut, you can see the stop.
I then made a pencil mark where the tile line was (I used a .25 overlap cut on the tile setup). I moved the board, registered the top holes to the dowels, screwed down the material, did a z probe, and nervously started the second cut. Here is a close up of the number "8" that was part of the tile...
And the tiled cut.....
IT'S PERFECT!!!! I was shocked. I thought I would be able to see a little edge or seam..... nope. It's perfect. I say that as amazement to the Vcarve tile feature and my cnc, not me.
Anyway.... wanted to share this registration technique with those trying to figure it out like I was.
Bill