Run through this before the drawing goes out. Each line is something I have seen add cost or scrap on a real part.
Geometry
- Inside corners have a radius, and it is larger than a standard end mill radius (not equal to it)
- Pocket depth is under about 4x the cutter diameter that fits the corner radius
- Thin walls are above 0.030" aluminum, 0.020" steel, and not tall
- No undercuts or features that need a fourth setup unless they are worth it
- Threads: standard sizes, depth no more than 1.5x diameter, drill point clearance allowed
Tolerances
- Default title block tolerance is realistic for the process (±0.005" is normal, ±0.001" is a decision)
- Tight tolerances are only on features that touch something
- Datums are on surfaces the shop can actually fixture on
- Tolerances do not stack across a chain of features that could be dimensioned from one datum
Material and finish
- Stock size chosen so the part comes from a standard bar or plate with minimal cleanup
- Finish callouts match the process (an as-machined 63 Ra does not need a note)
- Anodize or plate growth is accounted for on tight bores and threads
- Deburr and edge break called out once, not on every edge
Drawing
- Revision block filled in
- Material spec and temper named
- Quantity and any inspection level on the PO, not buried in a note
- Model and drawing agree; the model is the authority if they do not