Sure, but I’ll be totally honest and let you know that, once I had my model, I just followed a tutorial video on Vectric’s support website step for step, but I’ll gladly sum it up and provide the link.
http://support.vectric.com/tutorials/V9/selectedvideo.php?video_id=51
Once I had the model designed the way I wanted in F360:
-Go to Make>3D print.
-Select the model
-Ignore “Preview Mesh”
-Select High for “Refinement”
-Deselect “Send To A 3D Print Utility”.
It will then save it as a new .STL 3D model to wherever you choose to save it.
In VCarve Pro:
-Set up a 2-sided job, zeroing off the Material Surface (be sure to check “Zero Off Same Side” meaning you’ll set Z zero from the bed after you flip).
-Hit Ok
-Go to Modeling tab>Import a component or 3D model> select your .STL file
-Orient it within your work piece, Scale it (if need be) and Center Model in the work piece.
-Set Zero Plane Position in Model to the center
-Set the Overcut Distance to a little past half the depth of your work piece. This is so it will cut just past the center and not leave a seam. Most choose the radius of their ball nose, I chose the full diameter of mine just to be safe.
-hit OK
-Go to Clipart>Clipart>3D tabs and add your tabs. I chose 6 half-inch tabs but probably would have been fine with 4.
-Go to Drawing and add 3 asymmetrical holes the size of your dowels. (snug fit) I did two at the bottom, one at the top. This is how you’ll align the X any Y of the work piece when it’s flipped.
-Select all Tabs and Dowel holes>right click>Copy to other side.
That’s all for the initial setup, then you’ll go to the Toolpaths:
-For the Top side, in Material Setup, you’ll make sure to set Z zero at the top of the work piece, Center the model position in the material.
-hit OK
-My first tool path was a Profile toolpath for the dowel holes using the 1/4" EM. These will go in to the work piece. (1" deep)
-Second Tool path was a 3D Roughing Toolpath with the same 1/4" EM. (Machining Limit Boundary: Model, Boundary Offset: 0.25, Machining allowance: 0.04, Roughing strategy: Z level, raster Y, Ramp 0.5")
-Third Toolpath was 3D finishing with the 1/16" BN. (Machining Limit Boundary: Model, Boundary Offset: 0.0625, Area Machine Strategy: Raster)
-Hit Toggle Top/ Bottom Side
-In Material Setup, Z zero is now the machine bed.
-Set up the same three Toolpaths but this time the dowel holes are a separate toolpath file and go into the SPOILBOARD!
-3d Roughing and Finishing should be the exact same unless your model is Asymmetrical. Remember, Z zero is now set to the machine bed. (I keep saying that because I buggered it up)
A couple notes on what I learned:
-On the XXl, Z travel is about 3 to 3.25 inches. My workpiece was 2.625 inches thick, so I had to slide the router way up in the bracket and leave enough of the tool sticking out to go 1.375" deep.
-It also had to go all the way down to the bed and cut 0.5" deep. Any deeper and the Z carriage would have slid off the rails. I also had to take the springs off because their tension would have caused the Z axis belt to skip teeth on that far of a travel.
-No clamps were big enough to hold this so I screwed it directly into the bed away from my dowel holes. Double sided tape won’t work because unless you account for its thickness.
-Each side took about 4 hours with tool changes.
Hope this helps!