There is a need to draw a distinction between being able to use parametric modelling features and being able to model products in parametric modelling systems. This is to do with design intent. Design intent is a term used to describe how the model should be created and how it should behave when it is changed. With a parametric modeller it is very important to plan out the design before modelling. Design intent is built into the model according to how dimensions and relations are established. Changes to a model will yield a different result for each different design intent. Design intent is not just about the size and shape of features, but includes tolerances, manufacturing processes, relationship between features, dimensions, and the use of equations. Sketches should be dimensioned in a way that defines the design intent. It is quite easy to build a parametric model of a part that is fully constrained and looks correct, but from a practical viewpoint is useless. This is because the design intent for the part has not been adequately considered. The following examples help to clarify what is meant by design intent.
Examples of Design Intent
There are a number of ways of capturing design intent, the most important of which is dimensioning. Other methods of capturing design intent are through using relations and equations. Sketch relations or constraints such as parallel, horizontal, vertical and tangent and so on, can be incorporated into the sketch geometry, either automatically while sketching or added manually afterwards. Other basic examples of design intent in respect of features include, holes that are supposed to be through holes should be created so that if the thickness of a part changes, they will always go through the part, or holes that are centred on a circular boss should maintain this relationship if the boss is repositioned and so on.
There are usually several ways of building most parts and the choice of features and modelling methodology will also affect design intent. For instance, the adoption of a machining approach to solid modelling essentially mimics the way a part is manufactured by starting with a base feature that represents the stock material and then removing material with a series of cuts. Other approaches are the layer cake approach where a part is built up in successive layers of features, and the potterâs wheel approach where the part is revolved as a single feature. While the latter approach appears to be very efficient, having all the design information in a single feature can limit design flexibility. Ultimately the best approach will depend on the particular design requirements.
Capturing Design Intent in SolidWorks
There is no button to press for design intent. You build in design intent as you create each part. Remember it is your plan for creating the part model. So let's look at how to build in or imbed design intent.
Creating a sketch
- Create a rough sketch of the best profile on the most appropriate sketch plane. Imagine you had the part in your hand to help in deciding whether to place the first sketch on the Front, Top or Right plane.
- Capture relations automatically as you sketch and add in any extra relations if required.
- Add required dimensions to fully define the sketch (black).
Creating a Feature
- Create a Base Extrude, Boss Extrude, Cut Extrude, or Revolve feature, etc. from your sketch. Sweeps and Lofts require at least two sketches.
- Use the appropriate end condition for the feature. End conditions include Blind, Up to Next, Up to Surface, Midplane, Offset from Surface, Up to Body.
- Used to make dimensions equal to one another. Creates a bi-directional relationship between selected dimensions
- Use equations to add an algebraic relationship between dimensions. Creates a one-directional relationship between selected dimensions, viz. A=B, C=D, etc.
Ways of adding relations
- Automatic: When you draw a line and see the symbols H or V you are automatically adding a Horizontal or Vertical relationship to that line.
- Relations Icon: Select the Icon and choose the lines or arcs, etc. that you want to add relations between. Select the relation you want to add in the PropertyManager and select OK.
- Control Key: Hold down the control Key to select the geometry that you want to add a relation between. Relation options will automatically appear in the PropertyManager.