Standards of Completeness and Quality
· Sketches: Draw freehand with pencil on plain 8 ½ x 11 paper. Include title at the top, notes that explain your ideas and contributions, name of designer (you), your signature, and the date.
· All Working Drawings: Include formal title block and border (consider SolidWorks A (ANSI) Landscape Sheet Format). Title blocks include title, scale, author, checker and dates.
· Assembly Drawing(s): Include section, detail, ortho and/or iso views of exploded and/or assembled models as necessary to clearly show the parts and how they go together. Also, include balloons (on assembled and exploded views), a parts list and good trails on any explosion. The parts list should at least include Item number, Quantity, and a column to name custom parts and clearly specify standard ones. The names of custom parts must match titles given on part drawings.
· Part Drawings: Include all views and dimensions necessary to define the part geometry. Tolerance all dimensions to conform to stated minimum reasonable tolerances of relevant processes and minimum clearances vs. mating parts. Note material, and units.
· Drawing Set: Include an assembly drawing for each assembly and sub-assembly and part drawings for each custom part.
· Avoid Contradictions: Never use the decimal places of a dimension to round off a quantity. For example, if the length of a feature is 1.625, you should not allow its dimension to state 1.6.
· Dimension hole sizes and list characteristics using hole callouts (use quantity note to show # of common holes – ex. 2X). This requires the also desirable use of hole features to model holes (Hole Wizard or for bored/custom-size holes Insert/Features/Hole/Simple).
· Dimension a hole’s location by referencing a centermark or centerline.
· Place extension lines with visible ‘gaps’.
· Avoid multiple parts per drawing or multiple drawings per drawing file. Also, avoid multiple parts per part file. Some exceptions apply such as a family of similar parts where differences are specified with a table on the drawing.
· Give meaningful names to your computer files.
· Place dimensions off the views (i.e. not covering the picture).
· Place dimension text in the clear (i.e. avoid overlapping arrows, extension lines, etc.).
· Holes are tapped by modifying a hole feature (not by adding a thread feature).
· Where a part is symmetrical, indicate symmetry with a centerline and tolerance the symmetry with a note or a toleranced dimension (not as good but common). Alternatively, use a positional tolerance and a datum feature of size.
· If you’re stuck designing in English units, think in simple decimal sizes when you design (like 1.6), and use fractional sizes for stock and standard components only. When you use fractional sizes (like 1.625), dimension them with a fractional style (like 1 5/8 see Dimension Properties/Other Tab/Override Units/Fractions).
· Choose your sizes of stock or standard components by using, a manufacturer’s catalog (list of Component suppliers on Dept page) or from among the preferred sizes on this list from Columbia University’s Mechanical Engineering Department. If you choose a component from a Manufacturer’s catalog, include the relevant info (Company, part#, etc.) in your parts list.
· Where stock sizes are used on final geometry of custom parts, include stock dimensions but indicate that tolerances do not apply by including parenthesis or the STK suffix.
· Dimension holes in view looking down hole.
· Dimension outside diameters from the side (not in circle view).
· Avoid dimensioning to hidden lines (consider a section view).
· Avoid dimensioning to the tangent point of a radius.
· Model chamfers with a chamfer feature and dimension chamfers with a chamfer dimension (Tools/Dimensions/Chamfer).
· Avoid modeling very small chamfers or fillets/rounds (specify with note. Ex. “BREAK ALL EDGES .005 TO .010”).
· Avoid over dimensioning (saying the same thing twice).
· Apply geometric dimensions and tolerances where appropriate to lower manufacturing cost.
· Design and Tolerance consistent with process capabilities as stated in your design guide.
· Delete unused sketches (it’s easiest to kill them immediately).
· Avoid unused geometry in sketches.
· All reference geometry exists for a good reason.
· Specify part finish (using notes or symbols).