Tools/boxford/BoxfordQR

Introduction

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

Initial Tasks

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

Setups ⇒ New Setup.

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 ⇒ Model Box Point
		Model Point ⇒ Select point on model 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
Post Process		Nothing to set in here.

Facing Off

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

Tab	Setting	Details
Tool	Tool	Tool ⇒ Choose from library
		Coolant ⇒ Flood
	Feed & Speed	Spindle Speed ⇒ Max 3000 rpm
		Feedrate ⇒ Max 300mm/min
Geometry	Stock Contours	Stock Selections ⇒ Select the top surface of 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

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
		Pecking Depth ⇒ Depth for each cycle. 2mm is a good default.

2D Milling

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

3D Milling

Tab	Setting	Details

Chamfering

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

Setup the air compressor. Connect from the un-oiled port at 5 Bar to the Boxford inlet. Set the Boxford regulators to 1-3 Bar for the lower regulator and 1 Bar for the upper regulater. Drain any water from the regulators.

Power on the Boxford. Login to Fusion 360 and start CNC.js.

Machine Shutdown

Clean the inside of the machine and the table. Remove any mounting hardware. If the vice is mounted and trammed in, that can be left in place. Ensure the table and head are parked in sensible places. Log out of Fusion 360, and shutdown 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.