Guidance needed cutting 48" on Journeyman

I ran into a situation where I could not surface 48" of my spoil board. I was using Fusion360, and no setting I could find would allow the OF to surface 48" using my 1 1/8" surface bit. I had to reduce the size to 47 3/4". I tried cutting using various method in Fusion such as Pocket, Face, and Chain. I was able to position the cutter manually but not with the probe block. The probe block always told me I was “Under”. I was able to get it surfaced by manually positioning the cutter until I got no warnings. It left a small bit of uncut surface on the left side that I took down with a block plane. That being said, my real issue is going to be coming up and I need to know how to beat this. (As a side note, I used the 1 1/8" surface bit to cut all the way around the cutting area and it cut well out to over 49". I did this manually, but I could not replicate it using Fusion. The point is that I know that th ebit will cut that far.)

I picked the Journeyman because it supposedly has a 48"x32" cutting area. I want to be able to cut sheets of plywood and MDF that are 48" wide to cutout parts. So the guidance I need is how to use Fusion360 to setup a cut that can go 48". I plan to use a 1/4" carbide combination bit to do the cutting.

1 Like

Hey JonnyDex,

if you use a g-code toolpath created by a CAD/CAM software, and you have entered the correct limits of your machine, and the correct bit diameter, it will always subtract the radius of the bit (=half the diameter) at every end of the workarea, to force the bit to stay within the limits.

Of course, you could also go further out with the bit until it protrudes at the edge of the wasteboard, because there is still enough space there. But then you have to trick the CAD/CAM software. Either you make the workarea limits larger, or the bit smaller in the software settings.

The other method is not to use a g-code toolpath program at all, but to jog around with the gamepad.


Manually surfacing my waste board after it gets too chewed up is one of my simple pleasures in life, I have to say. Such a satisfying task.

1 Like

Yes, I like it too. The thing is, I used the spoil board as an exercise for learning to use my CAD/CAM program and the OF. I learned a lot but was left with questions I couldn’t answer. Aiph5u has hit the nail on the head I believe.


Thank you. I suspected that this is the case but you have more than confirmed it.

Write the surfacing toolpath for a smaller tool, then use a larger tool when you run it.

1 Like

I struggled with the same issue about a year ago. My memory was a bit dim, but fortunately I took good notes at the time.

Regarding the usable working area of a Journeyman:

  • Onefinity’s Journeyman specs give the “cutting area” as 48-1/4” (X-axis) x 32-1/4” (Y-axis). But these are actually hard mechanical limits. And on my particular machine, the specified Y-axis travel is overoptimistic by about 1/16”.
  • After making some exacting measurements, I was able to tweak the “zero backoff” stall-homing parameters and the motor soft-limit parameters on my machine just enough to eke out a usable working area of 1225.5 mm x 816.4 mm (48.248" x 32.146") on my machine, and still have adequate mechanical-travel margin to avoid hard-stop crashes. That’s just enough working area to be able to machine a precise perimeter on a 48" x 32" spoilboard using a 1/8" bit (and very light cuts).
  • All that was a PITA, and you have also to update the working area numbers in the post-processor file. But it’s doable, if you’re sufficiently motivated. As for me, in hindsight I’d probably settle for a slightly smaller spoilboard and working area.

As for programming a spoilboard-surfacing toolpath in Fusion, I unsuccessfully tried most of the canned toolpaths that you did. The problem appeared to be that they all insisted on approaching the area to be surfaced from the outside, and there’s just not enough machine travel for that to work.

I finally discovered that the “3D Flat” toolpath will do exactly what we want. Here’s what my toolpath looks like for a 1" surfacing bit, with the machining about half done (after starting in the center):

To configure the 3D Flat toolpath:

  • On the “Geometry” tab, select the spoilboard perimeter as the machining boundary, and select “Tool center on boundary” as the Tool Containment strategy.
  • On the “Heights” tab, the surface to be machined must be be between the Top Height and the Bottom Height, non-inclusive, or else the algorithm will miss it. So for the Top Height, I selected “Model top”, and specified an offset of 0.01".
  • On the Passes tab, I specified an Axial Stock to Leave of -0.01". That way, I can probe for zero at the top of the spoilboard, and then running the surfacing program will machine 0.01" off of the current spoilboard height.
  • On the Linking tab, I specified a Ramp Type of “Profile”, a ramping angle of 2 degrees, and a point near the center of the spoilboard as a Preferred Lead-in Position.

Backing up a bit, in the Fusion CAM setup I had placed the workpiece coordinate system origin at the top midpoint of the spoilboard. So before running the surfacing program, zero your machine at the correct matching position by manually moving it to the exact midpoint of it’s working area (per the absolute-coordinate position readouts on the controller), and then zero out the X & Y axes. To zero the Z axis, I used the touchprobe, but you could also use the piece-of-paper technique.

I hope that helps, or at least sheds some light on the issue(s).


Hey JonnyDex,

if you enter g-code manually into the MDI, you can access to the entire workspace of the machine (which is 1220 × 816 × 133 (160) mm on Journeyman). What you enter with a motion command is the position that the center of the bit will move to.

So if you enter a movement in machine coordinates (G53) from X=0, Y=0 to X=1220,Y=0, X=1220,Y=816, X=0,Y=816, and finally back to X=0, Y=0, you will have milled not only the border of the entire horizontal workarea, but also half a bit’s diameter outside of it.

G21 ; set metric mode
G90 ; set absolute distance mode
G54 ; select default coordinate system
G53 G0 Z0 ; rapid move milling motor upwards to Z home
G53 G0 X0Y0 ; rapid move bit to machine home

(insert moving to the right Z height here)

F100 ; select a feed rate
G53 G1 X1220Y0 ; linear motion to the given machine coordinate
G53 G1 X1220Y816 ; linear motion to the given machine coordinate
G53 G1 X0Y816 ; linear motion to the given machine coordinate
G53 G1 X0Y0 ; linear motion to the given machine coordinate
1 Like