Best Practice

[matt]

I view Best Practice as a set of suggestions that allows a group of wide experience level to work together. This generally caters to the lowest level, because if everybody can't use your models, you're in trouble. The more educated/trained your CAD users are, the more of these general suggestions you can ignore, relax, or customize. If you have all black diamond users, you should be able to do anything and get away with it.

Best practice varies by industry (surfacing, mold design, sheet metal, large assemblies, machine design, design for motion, weldments, electronics, etc, etc...) and by company.

But, if I were to venture a few:

- use explicitly trimmed sketches rather than the regions/contours/overlapping/untrimmed sketches. Contours/Regions may be easier, but the regions can flip easily when big changes are made

- name sketches, dimensions, features, mates especially when they will be used in design tables, equations, or to drive changes to the model

- consider using color to call attention to key faces, features or sketches

- Use the tools to replace sketch elements rather than just deleting and recreating sketch elements. This helps the software keep track of relationships

- If you use a layout sketch to drive the model, don't consume the layout under another feature because the layout needs to remain at the top of the feature tree. Use Convert Entities to copy elements of the sketch into another sketch.

- There are some bugs with the combination of Convert Entities and Trim, possibly related to selecting an entire face for Convert Entities, and then deleting some of the entities. This results in the sketch losing the trims that you created, and the feature and downstream features failing.

- sketches should use relationships rather than dimensions whenever feasible to help promote design for change.

- When you make references to other parts of the model, reach as far back to the top of the model as possible. This means select a plane instead of a sketch instead of an edge. SolidWorks loses references easily, and the more stable the entity, the less likely it will get lost.

- Remember the Derived sketch is a parametric copy that you can put/orient anywhere.

- 3D sketches are very powerful, but they can be very tricky to use and to fully define. They are valid to use, but make sure you use them correctly, and have a good reason for using them rather than a 2D sketch.

- Avoid using edges created by fillet or chamfer features as references for dimensions, sketches, mates, or anything else.

- fillet features are preferred over sketch fillets because tangent arcs can be difficult to manage in the sketcher

- it is better to make more fillet features with fewer edge selections because troubleshooting which edge is causing a problem can take time

- Be very careful about mixing in-context features, equations, configurations, and design tables. You need to establish one clear method for driving the model, and these methods often are in conflict.

- A revolved cut can replace multiple extruded cut, and a hole feature may be even more appropriate.

- If you find yourself cutting away a lot of existing material on a part, you might consider editing the existing features rather than creating new ones.

- Learning to edit and repair sketches and features in SolidWorks is time well spent. If you make many changes, you will need to edit and repair often.

- Don't use multiple bodies when you need an assembly:
- parts you want to reuse in other assemblies
- parts for which you want to use multiple instances in the assembly
- any time you want to use assembly motion
- any time you might want to insert one of the parts into another part to use as reference

- Do not create mates to in-context features or assembly features

- Do not create assembly features referencing in-context geometry (a plane offset from a face of part1 that references part2.

- Do not create multiple references (part 1 of assembly 1 references part 2 of assembly 1 and part 3 of assembly 2)

- Do not create circular references (part 1 references part 2, which references part 1)



... Ok, too many "thou shalt not"s. You get the idea. It's hard to write best practices. And we're not even talking about a specific type of design or a specific company yet...

[jcapriotti]

- Mate to faces/planes when possible instead of edges or vertices.

- When mating a component, all mates should be defined to one other connected component if possible. Less mate binding issues later and easier to troubleshoot.

- Do not create mates of a component to an instance of a component pattern if it can be avoided. Behind the scenes, "mategroups" still exist, even if they hid them from us.

- Create sub-assemblies from groups of static components if your product structure will allow for it. Avoid a flat tree if possible.

[DavidWS]

-Create turned parts (i.e. shafts and the like) with revolved features, not multiple extrudes stacked on top of each other.

-For the above, create the fillets, rounds, and chamfers as features, not in the sketch fillets/chamfers

-Use the Hole Wizard over Cut-Extrude

-Use simple sketches and multiple features over complex sketches/fewer features

-Create multiple features over one feature with multiple regions

-Link dimensions when reasonable

-Use Design Tables over Equations

-Use a layout part with sketches to drive your assemblies & parts

[Frederick_Law]

-Create turned parts (i.e. shafts and the like) with revolved features, not multiple extrudes stacked on top of each other.

-For the above, create the fillets, rounds, and chamfers as features, not in the sketch fillets/chamfers

-Use the Hole Wizard over Cut-Extrude

-Use simple sketches and multiple features over complex sketches/fewer features

-Create multiple features over one feature with multiple regions

-Link dimensions when reasonable

-Use Design Tables over Equations

-Use a layout part with sketches to drive your assemblies & parts

Agree and disagree.
When designing cylinders, I put everything in one sketch for same part. Rod, gland, cap, body, piston.
Put all parts sketch in Master Sketch. So I can see interference in sketch.
It's easier to locate and size all the groves: oring, wiper, gland in same sketch then in features.
I also add tolerance in sketch dimensions and use them in drawing.
Again easier to see which one is ID, OD with + or - tolerance.

That's was an air over hydraulic cylinder. So different tolerance on air and hydraulic side. Use shop air to get 3000 psi on hydraulic.

And I'm all equation. One dimension drive a few equations for features instead of 20 dimensions in Design Table.
Equation to drive mounting holes depends on length instead of table for number of holes and spacing.

[mattpeneguy]

0,0,0...model everything where it goes.

Mate everything to the origin and the pesky mate problems disappear.

Inferred above, but worth repeating, drive all external relations down the feature tree, never up (up is a good way to get circular references, which SW doesn't like).

[Glenn Schroeder]

0,0,0...model everything where it goes.

Mate everything to the origin and the pesky mate problems disappear.

That depends on the industry. I think you'd change your mind pretty quick if you were modeling guardrails or bridge parapets that were 75 to 100 feet or more long, with multiple components used dozens or hundreds of times.

[Frederick_Law]

I think you'd change your mind pretty quick if you were modeling guardrails or bridge parapets that were 75 to 100 feet or more long, with multiple components used dozens or hundreds of times.

Not really.

Did the catwalk behind the signs. Ladder, cage.
Most of the parts will be at 0,0,0.
Most subassemblies are at 0,0,0.
Patterned parts are not.
Part reused in other locations will not.
Of course nuts and bolts will not.