CNC Checklist

CNC Checklist

Toolpathing

    • 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

Machine setup

    • 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