SolidWorks Tech Tip: Sketches That Enforce Proportion

Sometimes a sketched feature is not intended to produce a particular dimension, so much as to create a chosen proportion.

The most obvious way to enforce proportionality between any two dimensions in SolidWorks, is to write an equation. Equations are powerful and useful, and they have their place. But we also teach that Geometric logic is more robust and more automatic than Numeric logic. There are plenty of times that you want to enforce a design aesthetic, or capture a proportional relation, that would benefit from solving dynamically inside the sketch restraints, instead of through an equation. And this is usually done in SolidWorks by way of dimensioning an ANGLE somewhere in the sketch.

The Tangent of an angle is the proportion of the Rise divided by the Run, so a fixed angle implies a fixed proportionality between the two legs.  The only trick to this method is deciding where in your sketch, the ‘legs’ of the triangle are, waiting to be used.

Consider the sketch below – we have a half-ellipse, with a desired proportion that the height should always be 1/3 the width.
SolidWorks sketch half ellipse with a desired proportion

If we set the Height to be the desired value, (1.3333 currently), then we add a construction line that documents that rise/run angle.

Dimension the angle as a DRIVING relation, and you can now set the H dimension to DRIVEN.
SolidWorks drawing half ellipse with angle as driving relation

Now as you change the Width dimension W, the height will always respond proportionately.  This is especially useful when creating sketches that will used in either a SWEEP or LOFT feature, as this will allow the sketch a degree of elasticity so that it can respond to Guide Curve controls.

More SolidWorks sketching tips & tricks are available on the CAPINC website.

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