Design Strategy Tutorials

Does anyone know any good tutorials that show problem solving, or approaches to designing an object using standard CAD tools? I'm not looking for "This is how you do a revolve in Solidworks" but "We need to create X. This is how we can accomplish it using revolve and some booleans". I know my way around my CAD of choice, and can generally model the simple stuff that I've needed so far, but there is a fair amount of brute force and inefficiency in my approach.

I'm sure some feature based tutorials fit the bill and that is fine, regardless of the application. But I'm also looking for something that has the feel of looking over the shoulder of an experienced designer and picking up some clever approaches to solving design challenges.

This is a potentially enormous topic. I've been working in my system of choice for a dozen years, but I'm still working out better and better ways of using it. Apart from copious bitter experience, it's hard to be specific without knowing what kind of CAD you're using (may not need to know which brand) and what kind of models you hope to make. Organic shapes in SolidWorks requires very different approaches than blocky parts in OpenSCAD.

Most of my learning has come from experience, discussion forums, and presentations at user group meetings. I don't know of any specific resource for generic CAD problem solving skills.

As Dale said this is really an enormous topic with no real straight answers.

I am a CAD designer and there are a few rules as to how you would model a part.

1) Method 1 is imagine you are making the part on a milling machine. First block it out, then add the details. So for a holed block you would shape the block, then machine the holes. Its a simplistic approach, but works well for basic parts. This method is also useful if you produce a drawing. Imagine how the machinist will make it and add dimensions that he needs at each stage. This way you don't miss a dimension.

2) For more complex models you use boolean cuts or additions. Commonly you make the blocks, then make a linked copy. You then assemble the linked copies in the finished part. This way its easy to isolate each part should it need modifying.

3) Try to produce a bushy history tree (using booleans etc) if possible, not a long linear tree. The model is more robust and doesn't fail as easily as there are less internal model dependencies.

4) When creating a part always use "most persistent geometry" when dimensioning sketches or extrusions. This means use origin coordinates or planes defined early in the history tree, not edges of the model or recently created surfaces. The model is less likely to fail when modified. A part modeled using method 3) above where all blocks are from an origin can only fail in the modified block or final assembly.

5) Always do fillets at the end of the model where possible. They fail most often so its best if they are at the end.

6) Give everything a descriptive name it makes thing easier.

Beside the milling approach, my personnal philosophy of design for parts more complex than a plate with a single hole is as follow :

- design the functional surfaces in their main direction and only that, iow hollow cylinder if I need a hole. The part here is disjoined.
- trim those in secondary directions as needed, eg the hole depth could be dictated by the bushing used
- add the connecting surfaces not dependant of the mean of production, eg welded prototype or casted part
- add the surfaces dependant of the mean of production
- only then, add trims, fillets and accessory surfaces


this allow maximum flexibility when doing changes.