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.