Help - Swept Profiles

Hi,

I don't recall having this problem before upgrading to SW2004SP3, can anyone
help.

Put simply I have a profile swept around an ellipse - no problem so far. But
when I create a drawing and section the part in order to dimension the
profile it seems it can't be done. When I click the dimension cursor on an
edge it hi-lites the whole perimeter of the profile and I get a message
saying 'the selected entity could not be converted into a line or a circular
arc'. Any of you wise-ones know the work around for this.

Regards .. Roger

 

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?

...

 

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
www.dimontegroup.com. Its really the way to go.

 

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