Fully defined
Dimensioned and constrained correctly. Every entity has a determined position and size, and nothing can move unexpectedly. This is the target state for any production model.
Frames of reference
Two coordinate systems
CAD systems maintain two coordinate systems, and knowing which one you are working in explains several otherwise puzzling behaviours.
- Model coordinate system (MCS)
- The reference frame in which the system stores model geometry in the part file. It is defined by the system, and its location and orientation in space cannot be changed by the user. The MCS is what defines the default sketch planes — top, front and right — and the default named views. It is orthogonal, defined by three mutually perpendicular planes intersecting at the X, Y and Z axes.
- Working coordinate system (WCS)
- The local frame of the active sketch. Within a sketch you work in two dimensions with the third coordinate set to zero; on exiting, the system transforms those working coordinates into model coordinates. This is the mechanism described in Part 11 that makes parametric representation independent of dimensionality.
Which plane is horizontal?
An MCS can be oriented one of two ways. In one convention the XY plane is horizontal, giving the top sketch plane and the top view. In the other the XY plane is vertical, giving the front sketch plane and the front view. Different systems make different choices, and this is a recurring source of confusion when geometry is exchanged or when a designer moves between packages. Establish which convention you are working in before deciding what "up" means.
Where geometry begins
Sketch planes
Sketch planes control part creation in three-dimensional modelling space. Every feature begins by selecting a plane on which to draw its cross section, and the sketch is the basis of everything that follows. Where a model needs several sketch planes, they are used one at a time: select a plane, create the sketch, finish the feature, then select the next.
Three default planes are supplied — front, top and right. Beyond those, two options exist. Any face of any existing feature can be opened as a sketch plane simply by selecting it. Or a new plane can be created as reference geometry, positioned by offset, angle, three points, or by reference to existing faces and edges.
Face or plane? The decision matters
Sketching on the face of an existing feature creates a dependency: the new feature is a child of the one supplying the face, and it will move, break or fail if that parent changes. Sketching on a default or created plane keeps the feature independent. Neither is universally right — a counterbore should follow the boss it sits in, so a face reference is correct; a mounting hole positioned from the part origin should not, so a plane reference is correct. The choice is design intent, as Part 06 develops.
The single most useful indicator
Sketch status
Sketch status is the geometric state of a sketch, and it takes one of three values.
Under-defined
Missing necessary dimensions or geometric constraints. Entities retain degrees of freedom. The sketch looks correct and will move unpredictably when something upstream changes.
Over-defined
More dimensions or constraints than required. The system flags the conflict explicitly, which makes this the honest failure — irritating, but visible.
Status is conveyed through colour, through text, and through a symbol beside the sketch node in the feature tree: a minus for under-defined, a plus for over-defined, along with a warning marker in the over-defined case. Most systems will allow a feature to be built on an under-defined or over-defined sketch. That permission is not an endorsement.
A working rule
Drive every sketch to fully defined before creating its feature. The cost is a minute per sketch; the return is that a model behaves predictably under every subsequent edit. Where a sketch resists definition, the usual cause is a missing relation rather than a missing dimension — look for the relationship you meant and have not stated.
Vocabulary
Sketch entities, construction and reference geometry
Entities
The entity set covers lines, rectangles in several construction methods, circles, arcs, polygons, slots, ellipses, parabolas, splines and points. Two are worth singling out. The spline is a general-shaped curve providing freehand sketching ability, created by clicking a sequence of points; its mathematics is the subject of Part 11. And sketch text can be placed on faces, curves, edges and sketch entities, where it is treated as modelling geometry and can be extruded or cut — quite unlike annotation text created in a drawing.
Construction geometry
Auxiliary geometry that assists in creating a sketch without generating material. Any sketched entity can be converted to construction geometry by setting its construction property, and converted back by clearing it. Points and centrelines are always construction entities, and construction geometry displays in the centreline style.
The canonical uses are an axis of revolution for a revolve feature, a construction circle on which to place a bolt pattern, and a layout skeleton that positions several features consistently. The last of these is significantly underused: a construction framework driven from the origin gives a whole sketch one governing set of parameters.
Reference geometry
Reference geometry is to feature creation what construction geometry is to sketch creation — part of the definition, not part of the resulting shape. Construction geometry lives on the sketch toolbar; reference geometry lives on the features toolbar. Planes and points are the most commonly used, with axes and coordinate systems next. Reference points are particularly useful as inputs to a curve, as Part 11 describes.
Holding geometry
Relations, equations and link values
A sketch relation is a geometric constraint between two sketch entities — horizontal, vertical, perpendicular, parallel, tangent, coincident, concentric, collinear, equal, symmetric, midpoint. Relations can be added while entities are being created or afterwards by editing the sketch. As you sketch, the system infers and displays the most plausible relation, which is convenient and occasionally wrong; inferred relations should be reviewed rather than accepted silently. The display of relation symbols is a toggle on the view menu.
Equations: driving and driven
An equation is a mathematical relationship between sketch entities, feature dimensions or other model properties, with parameters as its basis. Writing P1 = 2 P2 makes P1 the evaluated, dependent or driven parameter and P2 the independent or driving one. For the equation to evaluate, every parameter on the right-hand side must be known. Driven parameters cannot be edited directly — they are controlled by their equation — and only driving parameters can be changed.
Link values work similarly but more simply. They tie two parameters to a shared value, effectively an equality equation, so that changing one changes the other. Where the intent is simply that two dimensions must always match, a link value is clearer than an equation and easier for someone else to read.
Relation or equation?
Use a relation when the intent is geometric — these two lines must stay parallel. Use an equation when the intent is arithmetic — this length must always be twice that width. Substituting one for the other technically works and makes the model harder to read, which is the whole cost.
Speed and accuracy
Geometric modifiers and grids
A geometric modifier is a qualifier that selects a designated point on an existing sketch entity, and their value is that they remove the need to calculate coordinates by hand. They form part of what is usually presented as quick snapping.
End
Identifies the endpoints of an entity. An open curve such as a line has two distinct endpoints; a closed curve such as a circle has two coincident ones.
Centre
Identifies the centre or midpoint. For a line this is the midpoint; for a circle it is the point on the circumference at 180 degrees, not the circle centre — a distinction that catches people out.
Intersection
Identifies where two entities cross. Where more than one intersection exists, the system takes the one nearest the selection point.
Grids
A grid is an equally spaced set of points in a rectangular or radial pattern, rectangular being the more common. It has three parameters: spacing along the two axes, an origin, and an orientation. Grids speed construction and are particularly useful for sketches containing repetitive shapes.
Two points on grid behaviour. Displaying a grid does not enable snapping to it — display is a document property and snap is a system option, and both must be set. And grid lines are visible only while a sketch is open, which is frequently mistaken for the setting having failed.
Repetition as intent
Patterns
A pattern — also called a geometric array — is a uniform layout of a sketch entity or a feature in specified directions. Phone keypad keys and flange bolt holes are the standard illustrations.
| Type | Instances separated by | Typical application |
|---|---|---|
| Rectangular (linear) | Increments in the X and/or Y directions. | Vent slots, keypads, mounting-hole arrays on a plate. |
| Circular (angular) | Increments in the angular and/or radial directions. | Bolt circles, spokes, gear teeth, lightening holes in a disc. |
| Curve-driven | Distance along a defining curve. | Features following a non-linear edge or path. |
| Mirror | Reflection about a plane or centreline. | Symmetric parts — build half, mirror the rest. |
| Table or sketch driven | An explicit list of coordinates or a sketch of points. | Irregular but specified arrangements, such as a drilled hole map. |
Sketch entities and features can both be patterned, but not from the same place: patterning sketch entities requires an open sketch, patterning features requires being outside one. Choosing which level to pattern at is a design-intent decision. Patterning at feature level keeps each instance as a real feature that can carry a hole callout and be individually suppressed; patterning at sketch level is faster and produces a single feature.
Never copy what you can pattern
Four copied circles are four independent entities requiring four edits and offering four opportunities to be inconsistent. One patterned circle with an instance count of four is a single definition. The difference is invisible until the first change request, at which point it is the entire difference.
Working technique
Selecting, editing and measuring
Selection is required constantly — to edit entities, to reference them in new construction, to delete them — and the available methods differ more than they appear.
- Click an entity to select it.
- Hold the modifier key while clicking to build a multiple selection from scattered entities.
- Drag a selection window to capture many at once. Only entities fully enclosed are selected; partially enclosed entities are not.
- Right-click any entity in a connected run and select the chain option to take the whole run at once — used when selecting from sketches.
- The equivalent loop selection is used when selecting from feature faces. Chains and loops are the same idea applied at two different levels.
Measurement tools report distances, angles, radii and arc lengths between selected entities without modifying the model. Using them during construction — rather than inferring dimensions from the display — is the difference between knowing a clearance and assuming one.
Key takeaways
- The model coordinate system is fixed and defines the default planes and views; the working coordinate system is local to the active sketch.
- Sketching on a feature face creates a parent–child dependency; sketching on a plane does not. Choose deliberately.
- Drive sketches to fully defined; where a sketch resists, the missing item is usually a relation, not a dimension.
- Construction geometry belongs to sketches, reference geometry to features — both define without generating material.
- Relations express geometric intent, equations express arithmetic intent, and link values express equality. Use the one that reads correctly.
- Displaying a grid and snapping to it are two separate settings in two separate places.
- Pattern rather than copy, and decide deliberately whether to pattern at sketch level or feature level.
Series
Continue the pathway
The SOLIDWORKS Design Approach series works through computer aided design as an engineering discipline, from first principles to manufacture.
KEVOS®
Precision to Vision
Engineering · Mechanical Engineering
Written by Kevin Jogin
9 min read