CAD Checklist

"Rules of thumb" for the average model and drawing...

3D Models

The 3D model is the core of all subsequent drafting, design, manufacture, CNC programming, documentation. It is by far the the most important computer file relating to a manufactured item. Do it well!


  1. Use mm! Inventor > Metric template > Standard(mm).ipt
  2. PROFILE SKETCHES: It is good practice to use fully constrained sketches (profiles). You will gain a better understanding of sketch constraints and the model is much less likely to do strange things during an edit. It also means you haven't left off a dimension! In the real world not all sketches are fully constrained, but know the risks!  
  3. Never fix or undo a feature with another feature. This is bad. Instant fail. You must go back and EDIT the original feature (Right Button > Edit)
  4. Keep a clean history in the Browser Bar: No unused sketches. No invalid (red) features. No unnecessary features. Instant fail for any of these.


  1. FEW FEATURES: Try to get a balance between using the least number of features (compact Browser Bar history) and making sure features are easy to edit (each feature is a logical step). In other words, build the model in few steps, but without going overboard with complex or obscure shortcuts, or excessively complex profile sketches. 
  2. Parts designed for machining can often be modelled the same way as they will be manufactured. (E.g. Lathe parts are rotational extrusions). Likewise, sheetmetal parts usually reflect manufacturing. Parts for moulding or casting are pretty much random - model these however you like.
  3. SYMMETRY: Set up symmetrical parts centred on the XY,XZ and/or YZ planes. Comes in handy for mirror, assembly etc. See example of multiple mirror in highly symetrical part:Battery Holder
  4. Use Pattern or Mirror whenever you can save repetition. (Not only less features, but much easier to edit) 
  5. Leave small fillets (edge breaks), draft angles and finer or more trivial detail to the end. Fillets are often easier to do in 3D and  are left out of a 2D sketch so they don't complicate the dimensioning. For a large, complex model it helps to do fillets last because they slow down the processing - (fillets are mathematically complex.)    


2D Drafting 

Detail Drawings

The 2D drawings are generated from the 3D model. DO NOT draw lines yourself - they must be brouight in from the model
  1. Keep your 3D model and 2D drawing together (in the same folder). Never move them apart and do not rename them except through Inventor. (Otherwise when the drawing is opened in INventor it will not be able to find the 3D Model)
  2. Use mm! Inventor > Metric template > ANSI(mm).idw

    Third Angle Projection. You can also change any template to metric or 3rd angle (As per Australian standards 1100). To change Inventor to 3rd angle use Manage > Styles Editor > "Standard" > View Preferences > Third Angle. (See halfway through video Place Views)
  3. Keep number of views (projections) to a minumum. Three views is normal, the maximum (6 views) is extremely rare.
  4. Show hidden detail on all views (unless it is excessively confusing - where you might turn it off on an occasional view)
  5. Use correct paper size (usually A3) and select the largest scale that still allows room for dimensions.
  6. Add centre lines and cross-hairs to holes.
  7. Set BASE view : as the stated fron view, or select the most important, major view. This is often a side view (e.g. side view of a car would make a perfect "front view" to make as your BASE view in a drawing. All other views are projected off this base view.

2D Drafting (Assembly Drawings)

Rules are the same as for Detail Drawings (above) except...
  1. No dimensions unless absolutey necessary.
  2. No hidden detail unless absolutey necessary.


Rules for Dimensioning a Technical Drawing

  1. Each dimension should be given clearly, so that it can be interpreted in only one way.
  2. Dimensions should not be duplicated, or the same information given in two different ways, and no dimensions should be given except those needed to produce or inspect the part.
  3. Dimensions should be placed in the views where the features dimensioned are shown in true shape. This may require auxiliary views. (i.e. Dimension only to true lengths)
  4. In machine drawings, all units are assumed to be mm.
  5. No outline of the part should be used as a dimension line or coincide with a dimension line.
  6. Dimension lines should never cross other dimension lines. Dimension lines should avoid crossing extension lines. Extension lines may cross each other. Longer dimensions should be placed further to the outside. (to avoid crossing). Try to avoid long extension lines.
  7. Notes should always be lettered horizontally on the drawing.
  8. A dimension should be attached to only one view: extension lines should not connect two views.
  1. Avoid placing dimensions upon a view except when there is no choice, or it promotes clarity.
  2. Avoid dimensioning to hidden lines.
  3. Avoid a complete chain of detail dimensions; better to omit one. Otherwise, add REF (reference) of brackets to one detail dimension, or to the overall dimension. This allows tolerances to determine the omitted dimension.
  4. Dimensions should be given so that the machinist does not need to calculate, scale, or estimate any dimension.
  5. Dimensions should be attached to the view where the shape is best shown. 
  6. Dimension lines should be spaced uniformly throughout the drawing. Approx 10mm from the object, and 6mm apart.
  7. A center line may be extended and used as an extension line, but it is always drawn as a center line.
  8. Leaders can be any angle except vertical or horizontal.
  9. Dimension figures should be approximately centered between the arrowheads if possible.
  10. Is is better if extension lines do not touch object outlines (1-2mm), and extended a little past the dimension line. (1-2mm)
  11. In general, a cylinder or hole is dimensioned by its diameter (e.g. 24), an arc is dimensioned by its radius. (e.g. R12). Put these on the view where they are seen as circular arcs.
  12. Dimensions applying to two adjacent views should be placed between views, if convenient.



Relevant pages in MDME
Web Links
  • Google search:
  • INVENTOR tutorial. Get Started > Tutorials > 6. Drawings