Tools/boxford/BoxfordQR: Difference between revisions
imported>Stever |
imported>AndrewC |
||
Line 254: | Line 254: | ||
* Home the machine by clicking the "Homing" button which will home all 3 axes. |
* 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 |
** 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. |
** 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! |
** Taking a photo of the relationship between the work and machine axes positions may help you recover from a crash later! |
Revision as of 19:03, 28 September 2021
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 ⇒ Nothing - this will face all of the stock to the highest point 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
- (If you're using a superglue mount, start this first to allow 20 - 30 minutes to set)
- Turn on the Boxford and its monitor.
- Get the air compressor 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.
- 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
Select the toolpath in Fusion and save it as G-code.
--- Toolpath export changed in last version update on Fusion, review before completing this section ---
Load it in CNCjs and check the job looks sane in the preview window and by checking the Max and Min dimensions for each axis, remembering that the preview will be rotated 180 degrees
Install the correct tool in the Boxford. Touch off on the surface using the feeler gauge.
Set the Z height in CNCjs to the height of the feeler gauge, offset to the top of the stock. (Eg if using a 0.7mm feeler gauge and a 0.2mm facing cut has already been taken, set the Z height to 0.5mm)
If required, make an 'air pass' to test the job
- Set the machine to move to a known Z height clear of the workpiece.
- 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 tooling from the chuck and wipe clean the holder.
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.
Return all collets etc to the drawers under the machine.