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Drawing Standards

45 Engineering Drawing Best Practices


  1. Use official company templates for all files.
  2. At the beginning of modeling a part, take a little time to strategize an appropriate build sequence before diving in.
  3. Keep design intent and manufacturability/inspectability in mind when choosing the origin and orientation about which to model the part. An extrusion, for example, is best modeled with its profile on a base plane and its principle datum at the origin, not oriented to the product’s coordinate system.
  1. Strongly consider basing a part on initial layout sketches establishing the major driving dimensions of the part.
  1. Build sequence should progress from primary to peripheral in small, logical, orderly steps.
  1. Parametrically structure the model in a manner that best exemplifies the part’s basic geometry and function. This creates a model that can be parametrically edited and leveraged to new designs down the road with fewer blowups and less time input. For example, a wheel is by nature axissymmetric (a shape revolved about an axis)— a “circular extrusion” if you will— so the modeler should take an axissymmetric approach.
  1. Except where clearly inappropriate, start with an additive rather than a subtractive modeling approach (i.e. don’t start by creating an anonymous hunk of material). This generally results in a cleaner and more obvious expression of design intent.
  1. When modeling a complex symmetrical part, model half of it, and mirror at the last practical point in the build sequence.
  1. Place driving dimensions in layout sketches or in immediate parent sketches. Don’t hide driving dimensions in unexpected places.
  1. NAME THE FEATURES as you model, especially if the model will be complex.
  1. Group features into logical subgroups placed in informatively named folders.
  1. For multiple parts driven by a common geometry, a) create the simplest expression of the common geometry (usually a layout sketch) in a separate file and link/embed it into related part files; or b) build the related parts in a single part file as bodies, then save the bodies as parts, maintaining references to the parent file. Avoid long reference file chains and circular references between files.
  1. Give strong preference to solid modeling over surface modeling. Use surface modeling only where solid modeling is impractical.
  1. Fully constrain sketches. Dimensioned or geometrically-related elements are preferred over fixed elements, which are preferred over underdefined elements. This is especially important for “free form” features based on splines, etc.
  1. Keep sketches simple. Multiple features are to be preferred over a single feature defined by a sketch with dozens of relations.
  1. Where practical, avoid dimensioning to theoretical corners or other currently or eventually (because consumed) off-part datums.
  1. Think of geometric relations as “givens” and dimensions as “variables” or edit points in your model definition. Use equations, “Link Values” and/or “Global Variables”, construction geometry, and geometric relations to reduce dimension redundancies and make the part “smarter” and more stable, integral and editable.
  1. Always perform an interference check between mating and/or close-proximity parts, and translate components to avoid assembly crashes.
  1. Create “Mate References” where they would be helpful in automating mating of large assemblies (e.g. fastener groupings). Use company standard naming conventions.
  1. Tidy up; delete extraneous features.


  1. Use sensible subassemblies to simplify highly populated assemblies. “Insert New Subassembly” is very handy for this.
  1. When an assembly or subassembly has elements that contact an environmental feature such as a floor or wall, create Mate References or reference geometry for that contact.
  1. Create exploded views only on request.
  1. Give preference to multibody parts or other “bottom-up” modeling practices over assembly-based “top-down” modeling practices. If using top-down modeling as an expedient, sever links to the assembly and replace with internal parameters at the earliest appropriate opportunity.


  1. When assigning dimensions, be conscious of expression of design intent, accommodation of manufacturing processes, and accommodation of inspection (especially for process-sensitive or setup-sensitive parts). But give design intent priority. Chain or ordinate or baseline dimensions may be appropriate or not depending on design requirements. Choose carefully.
  1. Dimension drawings from “scratch” using associative dimensions. Do not import (link) dimensions from parts and assemblies into drawings. (Oftentimes appropriate dimensioning practices for 3d modeling are not ideal for drawings.)
  1. Create bidirectional editable property-linked text fields in title block. (Define Title Block)
  1. Use A or B size drawing sheets (portrait or landscape); use multiple sheets if necessary. All sheets for a drawing should be the same size for easier physical print management.
  1. Line fonts and colors: Visible lines solid, normal thickness, black; tangent lines solid, thin, black.
  1. Display hidden lines only if necessary for full definition or clarity. Selective hidden line display (Hide/Show), broken-out or sections, or additional views are preferred ways to display hidden features.
  1. Dimensions should always be placed outside of the object outline where possible. Always place shorter dimensions nearest to the object lines. Dimension lines should never cross other dimension lines. However, extension lines may cross each other. Dimensions should line up in chain fashion or be grouped together as much as possible. Do not duplicate/repeat a dimension, even with parentheses added.
  1. Complex geometries that are to be produced and (perhaps) inspected via digital means (CAM/CNC/CMM) in hard tools or parts may be specified by reference to a defining CAD file, a blanket profile or positional tolerance, and all appropriate datums. Example: “This surface shall be located within 0.1mm to either side of its basic surface as defined by the current revision of XXXX.STP, with respect to datums A. B. and C.” A surface finish tolerance should also be provided to control smoothness.
  1. Drawings should be identified by status in the space provided in the title block(preliminary or draft, released for tooling, released for manufacturing).
  1. Revision status shall be indicated by status designation and sequence: for preliminary or draft status, X1, X2, etc.; for Released for Tooling status, T1, T2, etc.; for Released for Manufacturing, A, B, etc.
  1. Revision symbol shall be a triangle enclosing the revision letter or number. All revised drawing features shall be designated by a revision symbol inleaders where helpful. Revision symbols must be placed in the view in which the revised element resides so that they move with the view when it is repositioned.
  1. Revisions shall be described in the revision block in a clear manner with historical context. E.g. “R0.5 was sharp; 2.25 was 2.19; deleted raised logo from end face.” Use a revision symbol with leader to indicate location of deleted features. Where necessary to reduce confusion, number individual revision items within the block and symbol (e.g. B1, B2) for easier correlation.
  1. Leave space for the revision block to expand. Place a revision block on Sheet 1 only, add notes to other sheets directing the reader to Sheet 1 for revision history.
  1. Dimensioning standards: except as specified otherwise in this document.
  1. GD&T shall be used only where necessary to adequately constrain part variances or where it is likely to reduce falloff while maintaining acceptable fit.
  1. Design and refer to functional gauges in place of difficult-to-inspect tolerances where appropriate.
  1. Invoke standards, where appropriate, in place of explicit tolerances (e.g. “Tube tolerances per current ASTM A513 for CREW steel tube except where noted otherwise”. Consider adding reference tolerances in parentheses where helpful.
  1. Drawing should be a complete and unambiguous expression of requirements. Notes are good; make requirements clear; clarity trumps convention!
  1. Archive obsolete drawing revisions in the Archive directory as 2D PDFs titled by part number and revision plus “obs” (xxxxx revX obsolete); mark the drawing status field in Properties (which links to title block) as obsolete, and also mark “OBSOLETE” conspicuously among the drawing views. Where an obsolete drawing revision specifies a defining CAD file as a geometric standard, the defining CAD file shall also be archived in the same manner.
  1. Current CAD files shall be titled by part number and revision and placed in the Active directory. Their unique presence in the Active directory identifies them as current revisions.
  1. Materials shall be fully specified on drawings, except for source-specific project-approved resin formulations or other lengthy material specifications which shall be referred to a separate revision-controlled Project Approved Materials manual.

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