A CNC setup sheet is the document that gives an operator the job, tool, workholding, offset, coolant, and inspection context needed to set up a job without guessing. It should be a controlled shop record after prove-out, not a replacement for the program, tooling data, machine manual, safety procedure, or first-article inspection.
This guide covers what belongs on a setup sheet and the formula context behind common speed/feed fields. The example ranges and formulas are planning context only. Current tooling manufacturer data, the machine builder documentation, the controlling drawing, and qualified shop review govern final parameters.
Why Setup Sheets Matter
Setup sheets serve three practical purposes:
Reduce setup search time. A clear setup sheet with tool list, fixture details, offsets, coolant, and notes keeps repeat work from requiring tribal knowledge.
Catch mismatches before cutting. A setup sheet that lists expected tool lengths, work offsets, feed mode, workholding, and first-article checks gives the operator a review point before the first cut.
Preserve proven process notes. New operators and future shifts can follow documented, verified values instead of relying on memory. The sheet should be updated when a tool, fixture, program, or inspection requirement changes.
What Belongs on a Setup Sheet
A complete setup sheet should include:
Header information: Part number, revision, material, stock size, operation number (Op 10, Op 20, etc.), machine assignment, program file name, and date.
Workholding: Fixture or vise type, jaw type (hard, soft, step), clamping pressure if applicable, and where the part sits in the fixture. A photo or sketch of the setup is worth more than a paragraph of text.
Work coordinate system: Where X0, Y0, Z0 are located on the part. "Center of stock, top face" or "front left corner, top face." Include the G54/G55 offset number used in the program.
Tool list: For each tool, list the pocket number, tool description (e.g., "1/2 4FL EM, 1.5 LOC, AlTiN"), holder type (ER32, CAT40, etc.), stick-out from the holder face, and the tool length and diameter offsets to expect. If a tool has a specific insert grade, list it.
Speeds and feeds: RPM, feed rate (IPM), and depth/width of cut for each tool. These should be the proven values from the last successful run, not theoretical maximums.
Coolant: Flood, mist, air blast, MQL, or dry for each operation. Some tools and materials are specific about this.
First-article dimensions: The critical dimensions to check on the first part, with tolerances. Include which measuring tool to use (calipers, micrometer, bore gauge, CMM).
Notes: Anything unusual. "Deburr edges before flip." "Check tool 3 for wear every 20 parts." "This material work-hardens, do not dwell."
CNC Job Setup Planning Sheet
Generate CNC job setup sheets with automatic speed, feed, and MRR calculations. Printable shop floor documents with chipload verification, workholding, and coolant notes.
Speed and Feed Fundamentals
Every cutting tool has two primary planning parameters: surface speed and feed. Formula pages from tooling manufacturers commonly express spindle speed as:
RPM = (SFM × 12) / (π × D)
Or the inch shortcut: RPM = (SFM × 3.82) / D, where D is cutter diameter in inches.
Milling and drilling feed:
IPM = RPM × feed_per_tooth_or_lip × effective_edges
Turning feed: turning is normally planned as feed per revolution for a single-point tool, so IPM = RPM × IPR. Do not multiply turning feed by an old flute count from a shared setup sheet.
Use tooling manufacturer data for the actual cutter, insert grade, material group, coating, holder, coolant, and depth of cut. Treat broad material ranges as placeholders until the selected tool data and shop conditions are known.
Chipload, Surface Finish, and Tool Life
Feed and tool life: Very low feed can rub instead of cut, especially when the chip is thinner than the edge radius. Very high feed can overload the edge, holder, spindle, or workholding. The right answer depends on the exact tool, coating, grade, material, coolant, engagement, holder, and machine.
Surface finish estimation for turning: A common theoretical turning screen is:
Ra = (feed² × 1,000,000) / (32 × nose_radius)
where feed is inches per revolution and nose radius is inches. This is geometry-only context. Insert wiper geometry, tool wear, runout, chatter, built-up edge, material, coolant, depth of cut, and measurement method can dominate the actual measured finish.
Coolant selection: Treat coolant as a process and safety choice. Follow tool manufacturer guidance, material requirements, SDS/shop procedures, machine enclosure limits, mist controls, and local environmental or safety rules.