Open VCarve/Partworks (CAD/CAM program)
Open PDF vector file
Job setup:
Material size: measure your piece, make sure you have room on the edges for screws/clamps
Material thickness: use calipers
Z Zero at top of material
XY Datum position remains in lower left corner
Deselect offset
In most cases, do not select “scale design with job size”
Click Ok
Transform and edit options are in left sidebar
Toolpath options in tab on right side of window (pin open):
Select toolpath operation (ex/ profile toolpath)
Start depth usually 0.0”
Cut depth: about 0.02” greater than your piece (to cut all the way through)
Make sure to select “show toolpath advanced options”
Tool:
Select appropriate tool (ex/ ¼” straight)
Ensure diameter is correct (ex/ 0.25”)
Pass depth: Vertical depth the tool cuts into the material per pass - should never be more than the diameter of the bit
Stepover*: Amount the tool overlaps it’s previous pass (horizontally) - the higher the number, the more it overlaps its last pass and the less new material is cut per pass (more important with pocket toolpaths) - ex/ 50% sufficient for profile toolpaths
Spindle speed*: Revolutions per minute (RPM) of the spindle - depends on the material (ex/ 12000 for ¾” plywood, MDF, OSB and other wood composites
Feed rate: How fast the tool travels in the x/y direction (horizontally) - Feed Rate (inches/sec) = RPM x # cutting edges x chipload / 60
Chipload is determined from Onsrud Feeds snd Speeeds website - select proper data sheet for your material, select proper tool using series number (left side of table, can be found on tool’s shank) and diameter; select middle value.
Plunge rate*: How fast the bit moves in the z direction - no faster than 0.5” per sec
Passes: Automatically determined (cut depth/pass depth, averaged) - usually do not change
Tabs: Keep cut pieces attached to sheet so they don’t move. Select “Add Tabs”, add length and thickness (ex/ 0.25”and 0.25”), select “3D Tabs” if cutting wood and chiseling out later. Click “Edit Tabs” and use cursor to add them manually.
Leads not required
Ramps: Ease the tool into the material, extending the life of the tool. Select “Add Ramps”, and select which type (ex/ smooth).
No need to adjust Order or Corners
Name toolpath
Preview toolpath
Save toolpath: .sbp
Save VCarve/Partworks file (workflow): .crv
*if filename is too long, the machine can't find the file. Keep .crv filename short
*Changes depending on material and/or tool type - check with staff before attempting metal, plastic, foam, cork, etc
Open Shopbot (CAM program)
Spindle warmup routine if you’re first to use the machine that day (ask staff)
Insert correct collet and tool
Large Shopbot only: Tools -> Spindle RPM Control (ex/ 12000)
Small Shopbot only: Set side Spindle Control Box to proper frequency (Frequency = RPM/60)
Clear bed
Secure material to bed
Zero x and y: Zero -> two axes (x and y)
Zero z-axis using a piece of paper. Paper should be able to move under the endmill but have slight resistance.
Turn dust extractor on
Safety glasses and hearing protection!
Cut Part -> select .sbp file
Spacebar to pause, red button for emergency stop