Help - Swept Profiles

It seems/seams like SW is unable to extract a silhouette or profile from the face so, you will have to manually get/reference a intersection curve or silhouette split the surface or make the sketch visible to dimension and workaround this?

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Roger wrote:

Roger

This is normal

You will have to add to your drawing view sketch points with a coincident relation to the profile, (and possibly construction lines, which you can subsequently hide), and dimension to those defined points. Otherwise SldWks cannot get a handle on where on the profile you want to dimension to. In the case of a sweep around an ellipse, the profile at any point other than the plane of the starting profile will be a spline, even if in theory it should be something more primitive, like a conic section. Even at the starting section, the cross section of the actual solid feature will have been approximated by a spline- the modelling kernel cannot mix analytic and algorithmic geometry (the former based on simple equations, the latter on NURB splines) Consequently there will be no "quadrant points" available as there would be for a circle or other primitive shape.

Sometimes its hard, but it is a good policy to predict the needs of the drawing while you are modeling. For instance, if at all possible, the sweep profile (the start/end of the sweep) should coincide with the section. This way you can just bring the dims from the profile into the drawing (using 'insert model items' on a feature by feature basis) and you can avoid all of the issues Andrew mentions. The same goes for sweep paths - put the path where the drawing/manufacturing dims belong. For some silly reason, a majority of files I see from the outside of my company have the sweep path go right through the center of the profile. If the part will be dimmed to its outside (bend radiuses for wire, for instance), then the path should be on the outside so you can model functionally and just bring the sketch dimensions into the drawing.

Gene Dimonte created a presentation for SolidWorks World about modeling functionally for the drawing. the powerpoint is available at

Hi Edward,

Coinciding the section with the 'start/end' of the sweep and 'inserting model items' did it, all the dimensions I needed appeared. Great thanks, now I can get on and earn some more $$$$.

Regards ... Roger

drawing/manufacturing