There are so many, Charity.
Always use fully defined sketches.
Create fillets and chamfers at the part level, not the sketch level.
Try to keep the origin at the center of the part.
Don't create features that can't actually be machined.
Create logical sub-assemblies.
Practice, practice, practice.
Don't use Toolbox (McMaster-Carr is your friend).
Don't activate all the toolbars. The 'S' key is the key to happiness.
Create, and use, standard templates.
Use the hole wizard.
A poster (jboggs) over at Eng-Tips.com posted this in response to a similar question:
a. Use standard templates, files, and SW settings.
2. Plan your work:
a. Where will it make sense to have the origin positioned? Having the main planes on one side of a symmetrical part just complicates using that part.
b. Build the part around features that will be important in its use or mating.
c. If a part is symmetrical, use mid-plane extrusions to keep the main planes in the center of the part.
d. If the part will have some center feature to its function, like a pivot point, build it with that pivot point at the origin.
e. Learn to use 2nd direction extrusions to keep the origin and main planes at the functional center of the part.
a. All sketches should be fully defined.
b. Apply relations and dimensions in a manner that minimizes work for future design changes.
c. Apply relations first and learn to use relations instead of dimensions where possible.
a. Default choice for Extruded Boss: Mid-plane.
b. Default choice for Extruded Cuts : "Thru to Next"
c. Learn to extrude from "Offset". This will prevent the need for numerous additional planes.
d. Learn to use non-merged features to create multi-body parts.
a. Do not use smart fasteners.
b. Learn standard Fastener labeling conventions.
c. Minimize number of assembly mates. Excessive or redundant mates just make assemblies unstable.
d. Learn to mate to part planes and temporary axes. For example, mating to the center of a slot.
e. Avoid using advanced mates (symmetric, width) wherever possible. Example: Width mates require massive internal calculations and lead to unstable assemblies. They can be avoided by mating to part planes or axes rather than surfaces.
a. Weldments should be parts, not assemblies.
b. Weldment drawings:
i. Use relative views to describe individual components where needed.
ii. Drawings of large weldments should show both "as welded" and "as machined" configurations.
iii. Remove tangent lines in all but 3d views.
a. Drawings should be complete, unambiguous, and as simple as possible.
b. Turn on hidden lines and tangent lines only when required.
c. Do not include unneeded views.
d. Keep fastener descriptions short and simple.
e. Place notes on the sheet, not in a view. This requires using "Lock Sheet Focus".
f. Fill in reference drawing info in title block where applicable.
McMaster Carr is easy, but not RoHS friendly. Toolbox works for us and really helps when we bring in assemblies from vendors.
Jeff's advice is sound for beginners. Follow it now. You should aspire to outgrow it.
Always use fully defined sketches. unless you don't need to
Create fillets and chamfers at the part level, not the sketch level. except when you need to
Try to keep the origin at the center of the part. keeps the OCDers off your back
Don't create features that can't actually be machined. but learn machining first
Practice, practice, practice. Oftentimes the hard way is the right way. Do it until it becomes easy.
Don't use Toolbox (McMaster-Carr is your friend). TOOLBOX SUCKS!
Don't activate all the toolbars. The 'S' key is the key to happiness. and 'U' and 'F'
Speed kills. The long road is usually faster over the life of a project.
Just a few things that come to mind, some mentioned in Jeff's post too.
If a part is symmetric, mirror. Sometimes at the sketch level, sometimes a body, or anything in between (features, faces, etc.).
Use patterns where applicable, sketches, features, parts. (Another good reason to use the Hole Wizard, it can be used to pattern components in an assembly.)
Use the library. Like patterns, once you've made something, be lazy, and use it over as much as you can, computers are really good at copying things. Also, copy and paste (or Ctrl click drag and release) will work with an astonishing number of things in SW.
Keep sketches and features simple and straightforward. It's good to make parts with a minimum number of features, but don't get carried away making sketches and features overly complex just to make the feature tree shorter.
Yes indeed, there are so many.
Can you specify some best practices for assemblies and mates?
These were very helpful! What about using patterns? Do you have any tips for this?
Since you specifically asked about assemblies and mates, here are a couple:
1. I've set up my assembly template with 3 axes, one at the intersection of each of the three primary planes. I use these for the direction for almost every Linear Component pattern. This works much better than using a part edge, since deleting or editing the part can lose the edge and cause the Pattern to blow up.
2. Try to avoid mating to a component that was inserted into the assembly with a Pattern. I don't think this is as bad as it was a few years ago, but it can still require numerous rebuilds to keep the assembly updated.
Avoid sketch patterns. Instead create a single feature or body, and then pattern it. Mirroring sketch entities, on the other hand, for the most part works well and I do it often.
Speaking of patterning, when you use the Pattern feature in a Part, "Features to Pattern" will be selected by default. If you're patterning holes, or a similar feature, that's fine. If you're patterning an extrude, revolve, etc. (a body), choose "Bodies to Pattern" instead.
I'll add a few:
1. Add X, Y, and Z reference axes to your model templates.
2. Add reference geometry generously to every model. Name each one and put it near the top of the feature tree whenever possible, right under the origin.
3. Use reference axes for any pattern, move, or other direction reference, rather than an edge, if possible.
4. Use reference geometry for mates.