Milling is easier than 3D printing. To get to know the H-Series, we will start by milling a pocket into a piece of plastic stock. ABS, Acetal, or PET are the best options for this project.

Prepping Stock

The stock should be flat on top, and large enough to mill a 5mm diameter pocket 5mm deep. Clamp the stock in the Standard Vise, double-stick tape it to a flat surface like the print bed (we will keep tool loads low in this case), or screw it down using one of the tooling holes in the Dovetail Bed. Here we have clamped it in a vise:

Using the probe, come down to the stock and probe the top surface. More details about using the probe and setting offsets can be found in this video. And specifically about using WCS, which is important below.

We will use a WCS to tell the machine where the top of the stock is. In this case, we will use the the G55 WCS and set the Z-offset to the previously probed value (here, 42.56mm). Click on the "Change to" button to activate the G55 WCS. Sanity check: the Z-value in Machine Status should now be 0, because in the G55 WCS, 0 is set at the top of the stock.

Plunge a Hole Manually

To get comfortable with the machine, we'll do a manual operation here. We will use a 1/8" Flat Endmill in Spindle 1. See the end of this page for changing or installing cutting tools.

OPTIONAL: you can take this opportunity to set the XY offset of the tool if that hasn't been done already. To do so, make sure the X and Y settings of the tool offset are 0, then proceed to the next step.

Bring up the Spindle tool, in this case Spindle 1. Jog X and Y to roughly the center of the block, and set the WCS X and Y so that this becomes X=0 Y=0. Always double check the Machine Position after setting the offset to make sure the axis you set is now at 0.

Turn the spindle on by typing in an RPM value (12,000 is good).

Jog slowly down to the surface of the block. You should be using Z0.05 steps near the surface. Sanity check: when the tool just contacts the surface of the stock, Z should again be 0 or very slightly negative. If not, the tool Z-offset is not correct and must be changed. 

Jog the Z-axis down approximately 5mm, in steps no greater than 0.5mm to plunge a hole into the stock, then jog up in Z to clear the stock and set the Spindle RPM to 0.

Optional: Here is where we would set the tool offset, by pulling up the probe, jogging it down into the hole, finding the center of the hole, and setting that location as the X-Y offset of Spindle 1. Details on that procedure can be found here. Also redo the X and Y WCS now, and confirm the Machine Position is at X=0, Y=0. (The previous 0,0 was defined where the tool was at the center of the block, with no tool offsets applied. Because we now have offsets applied, if we were to leave the WCS as it was, the tool would actually mill a pocket at the offset positions [roughly -6,-6, representing the distance from a tool centerline to the probe centerline]. The operator of the H-Series machine MUST understand the relationship between Absolute Machine Coordinates, Tool Offsets, and WCS. If this is not clear after this tutorial, please start or join a conversation about offsets in the Forums.)

Generating CAM Toolpaths

Now we will generate a toolpath for milling a slightly larger pocket, at the same location. In Fusion360, model the stock as accurately as possible, and put a hole in the center. Then in the CAM section (Manufacturing tab), start a setup and define the stock:

Stock mode can be either "From solid" or "Relative size box" with "No additional stock". The origin should match what we set in G55 before: at the top center of the block. In the Post-Process tab, type in a WCS offset of 2, corresponding to G55 (0 and 1=G54, 2=G55, 3=G56, 4=G57, etc)

We will make a 2D Pocket with the following settings (Fusion360 file is also attached below):

Some of the important settings:

• Tool
  • #1 - must match Spindle 1 (#2 would be Spindle 2)
  • 3.175mm (1/8") Flat Endmill
  • Flood on if you plan to run compressed air on this operation 
  • 10,000RPM
  • 300mm/min feedrate (keeping tool loads down for now)
• Geometry
  • Select the edge or bottom surface of the hole
• Heights
  • Bottom height -5mm from top surface (same as our manual plunge)
• Passes
  • Multiple depths
  • Limit roughing pass to 1mm depth
• Lead-in
  • Ramp = plunge

This gives us this toolpath:

Now we will post-process this with the H-Series Post. 

Sanity check: open the Gcode file, look for "G55" near the top, and that the file is calling the tool you want to use (T1). Also check to make sure the lowest Z-value is -5.00. This information tells you how far down the tool will go into the stock. Double checking these will save you from crashing the machine.

Final check: jog the machine to about where you would expect the cycle to start (in this case, right above the existing hole). Make sure it matches the Gcode file.

Upload and Start

Upload your Gcode file to the H-Series machine and go!