Best Practice
Posted: Mon Apr 05, 2021 4:05 pm
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...
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...