CAD Best Practices

Cad practices are vital to our performance as a team and will remain important in any career path that interfaces with CAD. The thing to remember is that although it might be faster and make sense to you to do things a certain way, you are not the only one interfacing with these parts, we need to review and validate our parts and other people will use them. Following these practices is a good way for everyone to be on the same page and set you up for success on your co-ops and career as a whole.

One thing that is touched on frequently in this list is conveying design intent of specific parts. Being able to discern the function of a part from it’s design is a difficult, but very necessary skill from both the designer and a reviewer.

Parts:

Sketches:

• All sketches must be fully defined

  • never ever ever click fix relation, or click the “fully define sketch” button

  • All dimensioning should convey design intent

    • If an feature (such as a circle or cutout) must be centered on another feature, utilize sketch relations, rather than defining it off of one side:

      Open

      

      using relations, will stay centered if outer dimensions are changed

  • relations are just as powerful as dimensions and they should be used in conjunction with everything else, every sketch should have a combination of the two

  • undefined sketches will show undefined in their title on the feature tree through a “(-)” mark or bottom right corner “under defined” there will be blue lines

Open

under defined

• overly defined sketches will often fail to propagate to features, they are shown as over defined through “(+)” or at the bottom right corner “over defined”

Features:

• it is preferred to have more simple features than singular complex sketches

  • easier to edit features as changing sketches can break upstream features and sketches

  • makes changes more discernable and easier to catalog for other users

• Feature type should convey the design or manufacturing method

  • revolves are a good thing to use for parts designed for the lathe as they are dimensioned in the same way you would turn a part

  • vis versa for extrude features

• Fillets should go at the end of the tree

  • use feature fillets rather than sketch fillets where ever possible

• ALWAYS USE HOLE WIZARD NOT CUT EXTRUDE HOLES

  • much better for everyone, gives auto values for tap sizes and clearance holes

  • can be adjusted for custom values

Overall:

• Name and organize your tree, it is possible to place tree items in folders and rename, rename to convey intent or what the feature is doing

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Assemblies:

Mating:

• never ever ever fix or lock mate items in an assembly

  • there is always a better way

  • except for lock rotation on concentric mates

• mating should convey design intent

  • if two items must be concentric, mate the according features as concentric

  • if a bolt is designed to take a lot of load, mate parts using the bolt

• its a good idea to float your first inserted part and mate it according to the assembly planes in the orientation it will exist on the car

Hardware:

• Add hardware to folders and pattern wherever possible

• check with your system about standard hardware sizing, and also bolt depot

• the mcmaster plug in is a good place to look for hardware models

• When adding hardware into assemblies

  • download part

  • break links (right click and break link)

  • suppress threads and knurling if possible

  • save as a solid works part INTO PDM

  • use the version saved to PDM!

• pattern hardware wherever possible

  • multiple pieces of hardware that align (bolts, nuts, heat sets, stand offs, washers, etc.) can be all include in the same pattern