Sketching
Basic Concepts
- sketch planes can be planes or planar faces
- sketch planes are infinite in size
- sketches have sketch entities, geometric relationships, and dimensions
- group functional items into the same sketch. Don't put everything into one sketch.
- choosing the best profile
- order of tasks for sketching:
sketch the geometry, close to final size
add geometric relationships
locate the sketch
add the dimensions
test the geometry
- pick first sketch so it creates the bulk of the part
- consider fully constraining entities - yes and no
- build it so related features change together, so we don't have to chase dimensions
- rough out sketches, then control with dimensions and relationships
- use feedback dimensions to get the sketch into the right ballpark
- push and pull to see what's still moving
- watch for sketch boogers easily generated with fast doubleclicks
- unlike drafting, do not put everything into same location
- use the dynamic feedback to tell if sketch entities are approximately the right size
- drag blue lines to a new location
- drag blue lines to a new location during troubleshooting to understand the constraints
- better to add geometric constraints before dimensions, so that the sketch will change predicatbly when dimensions are added
- watch the automatic relationships added while you're sketching. Understand what you are selecting.
- usually it's not necessary to use a snap grid, but can set it up if this would be helpful (say if lots of parts with similar whole number dimensions).
- on a sketch, the longer arrow of the origin is vertical, the shorter arrow is horizontal.
- it's better to have simpler sketch geometry and more features, than more complicated sketch geometry and fewer features. However, you can share geometry from complicated sketches over multiple features.
- when using trim and extend make sure you select on the right side of the midpoint, else you'll extend the wrong direction.
- to input dimension values on the fly, enable T>O>S>General>[x] Input dimension value.
Along the Way
- rename your planes: Front, Top, Right or X, Y, Z or Elevation
- locate the initial sketch plane carefully. It determines isometric display, determines how displayed in a drawing (can use predefined views)
- set the length of a line in the Property manager to drive the size of a feature without explicitly putting a dimension on it.
- what's so bad about underdefined sketches - when a part is released to manufacturing, the sketches within it should be fully defined
- add meaningful constraints. Don't add more constraints than necessary.
- underdefined sketches can be useful early in the design
- splines in conceptual sketches are often left undefined
- thin lines imply endpoint with more than 2 things coming out of it.
- dimension point to point versus line to point
- if you want to make construction lines symmetric to another, turn all but the symmetry one to solid lines, apply symmetry, then convert back to construction
- realize that splines are commonly left underdefined. If you need them fully defined, use the Fully Define Sketch tool.
- add a construction line tangent to end of spline and drive angle of that construction line to drive the spline
- consider three ways to create a symmetric spline:
sketch and mirror
create symmetric horizontal and vertical construction lines and have them drive the spline
sketch, mirror, then Fit Spline to create single spline
- reusing sketch information: make a single layout sketch with all the relationships and share it, or make a coincident plane and then convert entities
- scan in concept sketches and use them as a guide for modeling
- you don't need dimensions in a model, but it helps with parametric control. Also, model dimensions can be automatically transferred onto the drawing.
- use the property manager to edit multiple dimensions (length & angle) in one location
- use the Modify Sketch command to move, rotate, or scale a sketch. It maintains existing relations.
Techniques
- if you don't know a dimension value, don't just add it. See if there are other ways to define the geometry.
- quality and robustness of your model is directly determined by good sketching technique
- turn off automatic relationships with CTRL
- might not want to model monolithic features (e.g. everything in the same sketch), because that makes it difficult to use configurations later to simplify
- insert a Sketch Picture into a 2d sketch and then trace around it to model the part
- if you use Sketch Pictures for a trace, name the sketch to indicate the presence of a picture
- for sketch pictures best use sharp black and white images
- use multiple profiles & contours off the same sketch
- Use RMB-Contour Select Tool (on sketch or in graphics) to pick from several contours on a sketch
- overdefine your sketch for construction, then have software help solve it for better information
- learn tools such as Tools>Dimension>Fully Defined Sketch
- layout sketches are frequently used when creating complex models. These are sketch es uses for visual or parametric reference.
- dissolve a library feature (RMB) to turn it back into a sketch
- add tolerances and 3d annotations to the sketch so they're available in the model and the drawing
- understand the constraints and selection. For example to change the angle of a parallelogram don't pick the top edge, but pick the top two vertices.
- understand the constraints and selection. Dragging a circle edge resizes, dragging a circle centerpoint relocates.
- choose Tools>Sketch Settings>No Solve Move to be able to drag entities without solving for the relationships. This will allow you to break geometry on dragging.
- driven dimensions cannot overdefine a sketch. Use them for feedback.
