Drawing Standards Guide

The Purpose of Multiple Views

A machined part is a 3-D object; the drawing must translate that form into 2-D information the machinist can interpret unambiguously. Each view you place should add new information (shape, size, or relationship) that is not obvious in the others.

The Core Views Most Shops Expect

• Front (Primary) View – Shows the most characteristic outline of the part and normally carries the majority of the overall dimensions.
• Top View – Projected directly upward or downward from the front view; clarifies thickness and features hidden in the front.
• Right-Side View – Completes the orthographic set; shows depth features that are hidden or foreshortened elsewhere.
• Isometric (or Trimetric) View – Not used for dimensions, but gives the programmer/setup machinist an instant 3-D mental picture of the finished part. Mark it "FOR REFERENCE ONLY."
• Section Views – Sliced illustrations that expose interior cavities or stepped pockets. Use whenever a hidden feature would otherwise demand a forest of hidden lines.
• Detail Views – Enlarged circular/elliptical "call-outs" of small features such as chamfers, fillets, hole patterns, or intricate surface finishes.
• Auxiliary Views – Only when a critical face is angled relative to the normal projection planes and must be shown true-size for dimensioning.

Minimum-View Rule of Thumb

Two views can occasionally define a plate-like part; three orthographic views are generally the minimum for prismatic parts. Anything with angled faces, undercuts, or internal cavities usually needs at least one section or auxiliary. If a dimension cannot be measured with common shop tools from the views provided, you need an additional view.

Hidden Lines vs. Section Cuts

Excess hidden lines ("dashed-line soup") slow interpretation and invite mistakes. If more than ~30% of a view would be hidden lines, switch to a section view.

Orientation and Datums

Anchor every drawing to a consistent datum scheme (typically A|B|C). All views must be projected from the datum-oriented front view so that coordinate dimensions and GD&T reference frames remain coherent on every sheet.

Do's and Don'ts

Why Dimensioning Matters

Dimensions convert geometry into actionable numbers—tool-offsets, cutter paths, inspection limits. A clear, consistent dimensioning scheme shortens CNC-programming time, minimizes scrap, and anchors quality-control to the designer's true intent.

The Building Blocks

• Size Dimensions – Linear or angular values that define raw geometry: lengths, diameters, radii, chamfers, tap depths, angles.
• Location Dimensions – Distances that position features relative to datums or to each other.
• Reference Dimensions – Shown in parentheses; for information only, never inspected.
• Feature Control Frames (GD&T) – Symbolic blocks that combine tolerance and datum references for size, orientation, form, runout, etc.
• Notes & Call-outs – Thread specs, keyway standards (e.g., "KEYWAY PER ANSI B17.1"), surface finishes, or material removal limits.

Best-Practice Conventions

• Dimension FROM datums, not from other features, to prevent stack-up.
• Use baseline (ordinate) or polar dimensions for CNC-friendly XY or polar coordinate entry.
• Dimension each feature once and only once, in the view where its true shape is shown.
• For cylindrical features, express diameter "Ø" in the view where the circle appears; show depth with "↧" symbol or section.
• Show hole quantities as "4X Ø6.80 THRU" instead of repeating four individual call-outs.
• Put angular dimensions on an arc leader or between the radial centerlines—not off to the side.
• Keep decimals consistent: e.g., three-place (.000) for ±0.005 in, two-place (.00) for ±0.01 in.
• Convey tolerances by:
  • Title Block default (e.g., "UNLESS OTHERWISE SPECIFIED: .X ±.2 .XX ±.01 .XXX ±.005")
  • Direct bilateral limit (12.70 ± 0.05 mm)
  • GD&T frame (Ø12.70 A B | Ø0.05)
• Use local notes or flag notes for process-critical info: "BREAK SHARP EDGES 0.25 MAX," "NO BURRS >0.1."

Chain vs. Baseline Dimensioning

Chain (feature-to-feature) accumulates error. Whenever overall accuracy matters, start every location dimension from a single baseline datum or use ordinate dimensioning. Reserve chain only for non-critical patterns like decorative slots.

Integrating GD&T (When to Use)

• Form (flatness, cylindricity) when the function requires the entire surface to be uniformly tight, not just opposite points.
• Orientation (parallelism, perpendicularity) to guarantee assembly fit instead of relying on tiny angular values (e.g., "0.1°").
• Position – the workhorse for hole patterns; apply MMC/LMC modifiers to allow bonus tolerance and cheaper inspection.
• Profile – the "Swiss Army knife" for castings or complex surfacing where a composite tolerance zone is easier than dozens of separate call-outs.

Do's and Don'ts

Why Tolerances Matter

A nominal size is only an ideal. Every cutting tool, machine axis, and gage has finite accuracy, so you must tell the shop how much variation is acceptable before function or interchangeability is lost. Good tolerance selection balances:

• Functional performance (assembly, load capacity, leakage)
• Manufacturing capability (machine/process limits)
• Cost (tighter = more setups, slower feeds, more inspection)

The Vocabulary of Variation

• Dimensional Tolerances – Linear or angular limits, e.g., 25.00 ± 0.05 mm or 24.90 – 25.10.
• Fit Classes – Clearance, transition, interference ranges that control how mating parts slide or press together.
• Geometric Tolerances – Form, orientation, position, profile, runout (GD&T) that govern shape and location beyond simple size.
• Surface Texture – Ra, Rz, lay direction; affects sliding fits and sealing.
• Material-Condition Modifiers – MMC, LMC, RFS to link geometric tolerances to size for bonus tolerance.

Functional Fits: Picking the Right Bandwidth

Use a recognized fit system so the machinist, QC, and assembly techs all speak the same language.

How Tight Is Tight Enough? (Rule-of-Thumb Process Capability)

• Saw or flame-cut stock ±0.5 mm (±0.020 in)
• Manual mill/lathe ±0.13 mm (±0.005 in)
• Standard CNC ±0.025 mm (±0.001 in)
• Finish grind/hone ±0.005 mm (±0.0002 in)
• Wire EDM ±0.003 mm (±0.0001 in)

If your tolerance band is narrower than the process capability, expect special tooling, extra setups, or rejection risk.

Putting Tolerances on the Drawing

• a. Limit or ± Size: Ø25.00 +0.02/-0.00 (press fit)
• b. GD&T Frame: Ø25.00 A|B|C | ⌀0.02 MMC (locational control)
• c. Title-Block Defaults: state general values, then tighten only critical features.
• d. Surface Finish: "2.4 µm Ra ON BORE Ø25.00" — place the triangle symbol directly on the leader to avoid ambiguity.
• e. Projected Tolerance Zone: add Ⓓ symbol for studs or press pins that protrude through mating parts.

Tolerance Stack-Up Awareness

• Baseline/ordinate dimensioning reduces accumulative error.
• Use GD&T Position with MMC so bonus tolerance absorbs manufacturing drift without sacrificing assembly.
• Consider temperature: aluminium grows ~23 µm/m-°C; an H7/g6 fit at 20 °C may seize at 80 °C.

Surface & Geometric Coupling

A tight sliding fit needs BOTH:

• Size control (Ø20 H7)
• Cylindricity (⌀0.03) or Straightness so it doesn't bind.
• Surface finish ≤0.8 µm Ra so it doesn't gall.

State all three; leaving any out jeopardises performance.

Do's and Don'ts

Why Notes Matter

Even the best-detailed views and dimensions leave questions about material, finish, handling, or revision control. Notes consolidate those non-geometric requirements so the part emerges from the shop exactly as engineering intended—first time and every time.

Anatomy of a Robust Title Block

A well-structured title block is the machinist's "one-stop shop" for global requirements.

• Drawing Number & Sheet Count – unique ID; "1 OF 2" prevents missing pages.
• Part / Assembly Name – plain-language description.
• Material & Specification – e.g., "7075-T651 ALUMINUM PER ASTM B209."
• Finish & Coating – "ANODIZE PER MIL-A-8625 TYPE II CLASS 2, BLACK."
• Heat Treat – "HARDEN & TEMPER TO 32-36 HRC."
• Default Tolerances – e.g., "UNLESS OTHERWISE SPECIFIED: .X ±.2 .XX ±.01 .XXX ±.005 ANGLES ±0.5°."
• Units – "DIMENSIONS IN MILLIMETRES."
• Scale – "SCALE 1:2 (DO NOT SCALE DRAWING)."
• Mass/Weight – aids shipping and lifting plans.
• Finish Symbol Default – "SURFACE FINISH ≤3.2 µm Ra UNLESS NOTED."
• Revision & ECO Table – change letter, description, date, approvals.
• Sign-off Fields – Drawn / Checked / Approved initials & dates.

Manufacturing Note Categories (with common wording)

Organising Notes for Fast Consumption

• Number notes sequentially (1, 2, 3…) and use those numbers in flag balloons next to features.
• Keep general notes on Sheet 1; move lengthy process specs to a separate "Process Sheet" if they exceed ~⅓ of the page.
• Use CAPS for global notes, Sentence Case for local notes—consistent styles increase scan speed.

Revision Control Essentials

• Never overwrite a note—add a new revision entry so the paper trail survives audits.
• If a revision affects fit/function, call out "AFFECTS INTERCHANGEABILITY" in the ECO description.
• Grey out superseded views but keep them legible until final release for traceability.

Do's and Don'ts

Why File Formats Matter

The right file format ensures your design intent is preserved and can be efficiently processed by our manufacturing systems. Different formats serve different purposes in the manufacturing workflow.

Preferred Formats

• PDF for 2D drawings – High resolution, preserves formatting, universally readable
• STEP (.step/.stp) for 3D models – Industry standard, parametric data preserved
• IGES, DWG, DXF – Accepted with compatibility verification

Common File Submission Mistakes

• Low resolution or blurry images
• Missing views or dimensions
• Proprietary file formats not supported
• Hand-drawn sketches as primary files

Print this page and tick each box before you send a quote package or production release.

Complete Drawing Package Example

Why Machinist-Friendly Drawings Matter

Some drawing habits are common among engineers but can cause confusion, extra work, or even mistakes in the shop. Here are some tips to make your drawings more machinist-friendly:

Good vs. Poor Drawing Practices

Proper Dimensioning Methods

Why Tooling Considerations Matter

Even well-dimensioned drawings can create manufacturing headaches if they don't account for real-world tooling and material constraints. Here are some of the most common pitfalls and how to avoid them:

Stock Size Selection

Specifying a part size that matches a nominal bar or plate size (e.g., 1.000" x 1.000") may seem efficient, but to achieve clean, machined surfaces, we often need to order the next size up and machine all sides. Always allow for a small amount of material to be removed on each face.

Corner Radii Considerations

Internal corners in pockets or slots cannot be perfectly sharp due to the round profile of end mills. Always specify a minimum inside radius (e.g., 0.031" or larger) and avoid calling out "sharp" internal corners unless absolutely necessary. Larger radii are easier and cheaper to machine.

Length-to-Diameter (L/D) Ratio

Deep holes or pockets with a high L/D ratio (e.g., a 6" deep hole with a 0.125" diameter) require special long-reach tooling, which is expensive, prone to deflection and chatter, and may not be stocked. Try to keep L/D ratios under 5:1 for best results, and consult with your machinist for deeper features.

End Mill Corner Radii

Most end mills have a small corner radius (e.g., 0.015" or 0.03") rather than a perfectly sharp tip. When designing internal corners, specify a radius at least as large as the tool's corner radius, and ideally make internal corners larger than the diameter of the end mill that will be used. This allows the tool to "roll" through the corner smoothly, rather than plunging in and abruptly changing direction—a common source of chatter, tool wear, and poor surface finish.