Modeling
Basic Concepts
- ask if it does meet your design intent
- consider there may be more efficient ways to do it
- choose from the different modeling approaches: wedding cake, revolve it, machining
- wherever you have symmetry, you will need a centerline
- add centerlines to show how the model goes together. May not be needed if you turn on "show sketch relations"
- leave cosmetic fillets until the end
- create multiple fillets with the same radius in the same command
- make the larger fillets first
- fillet order is important because fillets create faces and edges that can be used to create more fillets
- fillet order is not important, but do the larger fillets first
- doesn't matter if you do chamfers or fillets first
- leave draft, chamfer, and fillets till the end of the model
- applied features are applied directly to the part and do not need sketch geometry
- rename new planes with a more meaningful name
- add features in order of importance. Create less important features near the end.
- use isometric views instead of normal to to make sure you know what you are selecting. You don't want unnecessary parent/child relationships.
Along The Way
- use part configurations to represent models in a simplified state
- assign material to the part, otherwise could use surfaces
- renaming features: no need if running solo, but helps the next guy
- add fillets are fillets in 3d, not as fillets in a 2d sketch
- choose logical names to organize your work and help others understand (edit) your model
- add file properties to help with future communication
- clean up the faces versus redefing the feature
- extrude through the part: 15 mm from top face is listed as 25 mm from bottom
- zero radius fillets can cause problems in manufacturing, so use with discretion
- use reference geometry to define and document important part and assembly entities
- create a sketch plane on a nonplanar face to help with feature construction
- use sketch driven pattern if you don't have regular positions
- use CosmosXpress for simple part analysis
- flex your components
- if multiple features use the same sketch face, create a reference plane (and rename the plane).
- use indent to smoosh a part into another
- can split a single body into multiples (say mouse shape into top and bottom design). Master part approach
- can join parts into single part (mostly for FEA if have contact problems)
- you don't need a sketch (2d or 3d) to draw a curve. Can use Curve>Curve Through Reference Points
- choose your references carefully. Think before you tie dimensions to an edge, a vertex, or a face, because references may disappear
- use rollback to analyze a design, whether your own or somebody else's
- a part with too many simple features can be difficult to manage in the browser
- a part with too many complex features can be inflexible
- add draft and shell vfeatures as your building the model early on because they affect faces
- consider orienting your model (front, right, top) how it will show on the drawing
- use patterns where you can as they create fewer features than building items individually. They're also faster and easier to edit.
- suppressing parents will suppress their children
- children are unsuppressed when their parents are unsuppressed only when "Unsuppress with Children" is set (Edit>Unsuppress with Dependents)
- parents are unsuppressed when a child is unsuppressed
- use equations to build intelligence into your model. For example control a feature to half the parts length, or adjust distance in pattern based on part size.
Even Further
- setback fillets are used when three filleted edges meet at a vertex
- use Setback Fillets for drawn metal to more accurately reflect the stretching of metal
- use a Face Fillet if you want to remove imperfections along an edge. Face Fillet will swallow the imperfections.
- sometimes it's better to apply uniform fillet with box select, then use FilletXpert to resize individual fillets
- two rules for lofting - pick the same spot on each profile, and make sure each profile has the same number of segments
- check the mesh lines on your loft to make sure the lines look nice (no bunch, twist, kink), to avoid problems downstream
- it is better to loft between faces than edges when creating solid lofts, because SolidWorks will use the edge to create a new face which could introduce small errors
- use deform to change a surface by point, curve to curve and surface push
- cam mates can have multiple entities, but is better to have a single spline profile. It's more natural like that.
- best practice to create the path and guide curves first that that the profile appears at the right point in history to apply Pierce relations to make the sweep work.
- best practice to sweep to outside of a curve, when possible, to avoid self-intersecting geometry.
- for master models, consider "Insert Part", "Insert into New Part", "Split Part" and "Save Bodies."
- master models can push bodies from the parent to the child, or pull bodies from the child to the parent.
- pushing bodies transfers the bodies, but not the features.
- push operations: Split, Save Bodies
- pull operations: Insert, Part, Insert into New Part
- if entities are co-planar (but on different sketches), they can be made symmetric
- understand that revolves cannot be solved if you have a single point on the centerline or if your profile crosses the centerline.
- there is no problem with features intersecting other features. There is a problem with a feature intersecting itself.
- understand how self-intersecting features can be created (e.g. sweeps with big radii along lines with small radii).
- create a spline through known points or through typed XYZ coordinates
- scaling a part does not scale the reference geometry
Techniques
- use Local Operations (by Edit feature, unclick "merge results") to control what features will be operated upon. After completion use Combine to put them back together.
- consider component part with several default configurations: full, simplified (for location, mating), drawing
- suppress anything not required for mating, motion, interferences in a configuration
- consider maintaining external references (like lines and edges)
- make fillets and parts contrasting colors. Can automatically set all fillet features to be a different color.
- you don't need a sketch (2d or 3d) to draw a curve. Can use Curve>Curve Through Reference Points
- pattern linearly not just in X and Y, but X and -X
- for parts used in cryogenic environments, consider using two configurations (293K, 100K or room temperature, operating temperature) and using scale to resize the part due to temperature changes. Scale factors will be different depending on the material used.
- offset from surface versus translate from surface
- use tools>dimensions>fully define sketch
- Insert>Cut>With Surface vs Model the Right Sketch
- be aware of "merge solids" during mirror to avoid multibody problems
- use RMB-ParentChild to click on entities to edit. Check that parent-child relationships get corrected. This is useful prior to a reorder.
- realize that patterns (& mirror) do not support Sweep With Guide Curve unless Geometry Pattern option is used. A better approach is to create disjoint body, mirror body, then merge.
- store section view with model for use in drawing
- insert a gusset feature in any multibody, not just weldments.
- edges that may be filleted are bad references
- when several features attach to the same entity, use references for better control
- you can assist with renaming features by enabling T>O>S>FeatureManager>[x]Name feature on creation
- turn off and suppress fillets during the design phase to improve performance. However, make sure you don't add features dimensioned to edges that are filleted (and suppressed).
- enable dynamic editing during initial design phase to quickly move, rotate, scale features around the part.
