Tools/boxford/BoxfordQR

From rLab Wiki
Revision as of 04:48, 27 November 2021 by Stever (talk | contribs) (→‎Running a Job)
(diff) ← Older revision | Latest revision (diff) | Newer revision → (diff)
Jump to navigationJump to search

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

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.

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

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

"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

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

"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

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

  • (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

  • 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

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

  • 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.