Tools/boxford/BoxfordQR

From rLab

⚠️ This page is intended only as a quick reference guide for trained users! ⚠️

Introduction[edit]

A Quick Reference to generating a CNC toolpath from Fusion 360 for the Boxford and running it correctly.

Initial Tasks[edit]

Design the model in Fusion. Switch to Manufacturing mode. Open the tool library model in another tab.

Setups ⇒ New Setup.

Setup axis for the Boxford compared to the Fusion 360 View Cube
Tab Setting Details
Setup Machine Machine ⇒ Boxford 260 VMC
Setup Operation Type ⇒ Milling
Work Coordinate System (WCS) Orientation ⇒ Select Z axis & X Axis
Touch off on faces perpendicular to Z and X axes
Flip X-Axis ⇒ On
Origin ⇒ Stock Box Point
Stock Point ⇒ Select point on stock as origin. Top Centre is a good default
Stock Stock Mode ⇒ Fixed Size Box
Set width, depth and height, and the relative location of the model to each. 'Center' is a good default for X and Y
Z-Axis Model position ⇒ Offset from top
Z-Axis Offset ⇒ Depth of facing cut, zero if there isn't one
Post Process Nothing to set in here.

Facing Off, for preparing stock[edit]

Facing off Stock to bring it to a flat and accurate height

From '2D Milling' menu, select 'Face'

Tab Setting Details
Tool Tool Tool ⇒ Choose from library
Coolant ⇒ Flood
Feed & Speed Spindle Speed ⇒ Max 3000 rpm, keep to 2500rpm if possible
Feedrate ⇒ Max 300mm/min
Geometry Stock Contours

Stock Selections ⇒ Nothing - this will face all of the stock to the highest point of the model.
OR
Stock Selections ⇒ Select the top surface of the model - this will only face the area above the model.

Heights Defaults should be good. May adjust the Clearance and Retract heights to save time
Passes Passes Pass Direction ⇒ Angle offset from X Axis
Pass Extension ⇒ Distance past the face to extend for an overcut - X axis only
Stock Offset ⇒ Distance past the stock to move past for an overcut - Both X and Y Axes
Stepover ⇒ Overlap between passes. Do not use exactly 1/2 or more than 1 x tool width.
Direction ⇒ Use Climb milling, or both.
Multiple Depths Maximum stepdown ⇒ Depth of each pass
Both Sides ⇒ Cut in both directions on multiple passes
Finishing Step ⇒ Select to make a final finish pass
Finish Feedrate ⇒ Max 300mm/min
Finishing Stepdown ⇒ Depth of final cut
Stock to Leave Option to leave a margin on the facing cut for future operations.

Drilling[edit]

"Drilling - rapid out" for shallow holes, "Deep Drilling - Full Retract" for deeper holes

From 'Drilling' menu, select 'Drill'

Maximum drill size is around 6mm.

Tab Setting Details
Tool Tool Tool ⇒ Select from library
Coolant ⇒ Flood
Feed & Speed Max 3000rpm, 100 mm/min plunge rate
Geometry Geometry Selection Mode ⇒ Faces or Points. Usually Faces.
Hole Faces / Points ⇒ Select locations.
Heights Bottom Height From ⇒ Hole Bottom
Offset ⇒ How far past the bottom to go
Drill Tip Through Bottom ⇒ Select to make the entire hole full diameter
Cycle Cycle Cycle Type ⇒ "Deep drilling, Full retract" for holes more than 2 x drill diameter; "Drilling - Rapid out" for less than 2 x diameter
Pecking Depth ⇒ Depth for each cycle. 2mm is a good default.

2D Contour Milling, for cutting something out[edit]

Contour cuts can cut things out, using tabs to retain the part

From '2D Milling' menu, select '2D Contour'.

Tab Setting Details
Tool Tool Tool ⇒ Choose from library
Coolant ⇒ Flood
Feed & Speed Spindle Speed ⇒ Max 3000 rpm
Feedrate ⇒ Max 300mm/min
Geometry Geometry Contour Mode ⇒ Selected Contours
Contour Selection ⇒ Select the contour to mill
Stock Contours Used to calculate clearance for lead in and out
Tabs Tab Shape ⇒ Triangular
Tab Width ⇒ in mm
Tab Depth ⇒ in mm
Tab Postioning ⇒ By distance or specific points. Use points.
Tab Positions ⇒ Select locations on model.
Heights Defaults should be good. May adjust the Clearance and Retract heights to save time
Passes Passes Sideways Compensation ⇒ Leave on Left. Can compensate for tool wear etc.
Finish Feedrate ⇒ Max 300mm/min
Stepover ⇒ How far to cut each finish pass as you approach the final contour.
Both Ways ⇒ Leave unticked. Use climb milling.
Roughing Passes Maximum Stepover ⇒ Do not use exactly 1/2 or more than 1 x tool diameter
Smoothing Deviation ⇒ How fine to cut radii
Number of Stepovers ⇒ How many intermediate cuts to make to approach the final contour
Multiple Depths Maximum Roughing Stepdown ⇒ Max depth of each pass
Finishing Stepdowns ⇒ Number of cuts at finishing speeds
Finishing Stepdown ⇒ Depth of each finish pass
Smoothing Option to simplify G-code for curves
Linking Linking Leave on defaults
Leads & Transitions Lead-in ⇒ Select to use a lead-in path
Horizontal Lead-in Radius ⇒ Distance from side to approach
Lead-Out ⇒ Select to use a lead-out path
Same as Lead-In ⇒ Use the same settings for the lead-out
Ramp Enable to cut in a spiral path down to final depth
Ramping Angle ⇒ Keep shallow. Max 2 degrees
Max Ramp Step ⇒ Max depth of a single spiral cut
Ramp Clearance Height ⇒ Height above the surface to start the ramp down
Positions Predrill Positions ⇒ Select holes in the material for the tool to enter
Entry Postitions ⇒ Select locations on the job to for the tool to enter

Other useful 2D toolpaths

2D adaptive clearing : For removing spare material

2D Pocket : For recesses with flat bases

Trace or Engrave : For engraving patterns or text on a surface

3D Milling[edit]

"3D Adaptive Clearing" is good for complex 3D shapes

From '3D Milling' menu, select 'Adaptive Clearing'.

Tab Setting Details
Tool Tool Tool ⇒ Choose from library
Coolant ⇒ Flood
Feed & Speed Spindle Speed ⇒ Max 3000 rpm
Feedrate ⇒ Max 300mm/min
Geometry Geometry Contour Mode ⇒ Selected Contours
Machining Boundary ⇒ Select the outer limit of area to be cleared, or leave "nothing" to machine entire part
Stock Contours Used to calculate clearance for lead in and out
Rest Machining Source ⇒ From stock for first operation, from previous operation for subsequent ones
Adjustment ⇒ ignore cusps
Adjustment Offset ⇒ material to leave
Model Specify what model to use if there are several
Heights Defaults should be good. May adjust the Clearance and Retract heights to save time
Bottom Height ⇒ Can limit how deep to machine
Passes Passes Machine Shallow Areas - Add extra Z-steps when needed for shallow slopes
Optimal Load - How much of the width of the tool to keep engaged with work
Both Ways ⇒ Leave unticked. Use climb milling.
Machine Cavities - Go down into pockets within the shape
Direction - Which operation type to prioritize for horizontal moves
Roughing/Fine Stepdown - Size of large and small vertical steps to take
Stock to leave Radial Stock = How much stock to leave on sides
Axial Stock = How much vertical stock to leave
Multiple Depths Maximum Roughing Stepdown ⇒ Max depth of each pass
Finishing Stepdowns ⇒ Number of cuts at finishing speeds
Finishing Stepdown ⇒ Depth of each finish pass
Smoothing Option to simplify G-code for curves
Linking Linking Leave on defaults
No-Engagement feed rate - Maximum 300mm/sec
Leads & Transitions Horizontal Lead-in Radius ⇒ Distance from side to approach
Vertical Lead In Radius ⇒ Distance from top to approach
Ramp Enable to cut in a spiral path down to final depth
Ramping Angle ⇒ Keep shallow. Max 2 degrees
Max Ramp Step ⇒ Max depth of a single spiral cut
Ramp Clearance Height ⇒ Height above the surface to start the ramp down
Positions Predrill Positions ⇒ Select holes in the material for the tool to enter
Entry Postitions ⇒ Select locations on the job to for the tool to enter

The other 3D paths are for finishing operations once Adaptive Clearing has removed the bulk

Chamfering[edit]

Chamfer cuts are good for deburring and creating soft edges

From '2D Milling' menu select '2D Chamfer'

Tab Setting Details
Tool Tool Tool ⇒ Select from library
Coolant ⇒ Flood
Feed & Speed Spindle Speed ⇒ Max 3000rpm
Feedrate ⇒ Max 300mm/min
Geometry Geometry Contour Selection ⇒ Choose contour to chamfer
Heights Default settings should be OK
Passes Passes Leave at defaults
Chamfer Chamfer Width ⇒ In mm
Chamfer Tip Offset ⇒ Height above tip to use for cutting, in mm
Smoothing Option to reduce G-code load for curves

Machine Setup[edit]

  • (If you're using a superglue mount, start this first to allow 20 - 30 minutes to set)
  • Turn on the Boxford and its monitor.
  • Setup the air compressor and get it charging.
    • Set the regulator on the un-oiled port to 5 bar (0.5MPa, 70PSI)
  • Check the Boxford is reasonably clean. The bed and spindle must be spotless.
  • Login to Windows, start Fusion 360 and CNC.js.
  • Operate the one-shot oiler on the top left of the Boxford.
  • Connect the Boxford to the compressor using the un-oiled port.
    • Set the oil metering pressure (top regulator) to 1 Bar (0.1MPa, 15PSI)
    • Set the air jet pressure (lower regulator). Aluminium needs the highest pressure, brass the lowest; steel is similar to brass. The normal range of pressures is 1-3Bar (0.1-0.3MPa, 15-45PSI). Lower pressure means less swarf clearance, higher means you may overheat the compressor on longer jobs.
    • Empty the water drains on both regulators.
  • Log in to Fusion 360 and load your design.
  • Mount your work piece into the Boxford!

Using CNCjs[edit]

  • If CNCjs starts in an 'Alarm' state, follow the E-Stop procedure.
  • Check the bed and spindle are clear to move.
  • Home the machine by clicking the "Homing" button which will home all 3 axes.
    • The CNC milling machine has a maximum travel of 250mm x 130mm and a vertical travel of 180mm
  • Using manual movement, zero your work X and Y axes according to the Origin/Stock Point you set in your Fusion 360 setup.
    • This will often be the top centre of your stock.
    • Taking a photo of the relationship between the work and machine axes positions may help you recover from a crash later!


E-Stop

If the machine E-Stop has been pressed, clear the problem and reset the E-Stop button. Then use the 'Reset' and 'Unlock' buttons in CNC.js to regain manual control.


Manual movement

Set a movement rate in the 'Move' box. This is the value (in mm) that each axis will move for one keystroke, tap the keys, DO NOT HOLD THEM DOWN.

  • Left / Right Arrows move X Axis
  • Up / Down Arrows move Y Axis
  • Page Up / Down move Z Axis
  • Shift moves at 10 x speed
  • Alt moves at 1/10 x speed

Running a Job[edit]

The post dialog
  • Export the g-code for the cut from Fusion 360:
  1. Right-click the toolpath and click 'Post Process'
  2. In the pop-up window set:
    1. 'Post' to 'Boxford Smoothie.cps'
  3. Hit 'Post'
  4. Save .nc the file somewhere - probably to a folder with your name.
  • Import the .nc file into CNC.js by pressing the big blue 'Upload G-code' button.
  • Sanity check the job:
    • Look at the preview window (remembering that it will be rotated 180 degrees).
    • Review the Max and Min dimensions for each axis.
  • Install the correct tool in the Boxford.
  • Touch off on the surface using the feeler gauge.
  • Set the Z-height work axis in CNCjs to the height of the feeler gauge, offset to the top of the stock.
    • E.g. if using a 0.7mm feeler gauge and a 0.2mm facing cut has already been taken, set the Z height to 0.5mm.
  • Double check that you have actually set the z-height correctly.
  • Point the air blast at the tool.
  • Run an air pass (see below) if desired.
  • Click the 'Play' button.
    • Check that you've loaded the correct tool and set the z-height.
    • Press OK.
  • Click the 'Play' button (again).
    • Check that you've loaded the correct tool and set the z-height (again).
    • Watch it like a hawk with your hand over the E-stop if this is the first time you've used this .nc file. Second and subsequent runs you must remain next to the boxford but don't have to watch it constantly
    • Press OK.


Running an air pass

  • Set the machine to move to a known Z height clear of the workpiece, record/remember this height.
  • Set the Z height value to zero
  • Run the job and watch to check it runs as expected
  • Move the machine Z height back to the original value
  • Set the Z height value back to the height above the stock

Machine Shutdown[edit]

  • Remove any mounting hardware. If the vice is mounted and trammed in, that can be left in place.
  • Clean the inside of the machine and the table.
  • Remove any tooling from the chuck and wipe clean the holder.
  • Ensure the table and head are parked in sensible places.
  • Log out of Fusion 360, and shut down the PC. You will need to power off the Boxford as it tries to reboot after shutdown.
  • Empty the fluid drains on the two air regulators, and disconnect the air compressor.
  • Drain the air tank and put the compressor away.
  • Return all collets etc to the drawers under the machine.