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Help with sweeping lip along 3D sketch?

Hi,

I'm having problems sweeping a lip along a 3D sketch created from the edge of a part I am modelling. Although it looks a pretty simple thing to achieve I can't seem to get it to merge fully with the part and have tried loads of different methods.

I've posted some screen caps and the part file at the following address instead of trying to explain it all in words.

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Perhaps it just isn't possible with the profile I currently have?

If anyone can give me any pointers that would be fantastic.

Many thanks,

Tom

Reply to
tomcrick
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your path has "convex" corners and small radius filets which would cause self-intersecting geometry. You have to do multiple sweeps along each section of the path. Composite curves are handier than 3D sketches to do this:

1) create a composite curve with a sinngle segment of your path 2) create a normal plane to it, sketch your lip profile 3) do the sweep along the composite curve 4) add segments to the composite curve and rebuild until you can't go further 5) create a new composite curve with next segment, normal plane 6) insert a "derived sketch" of your profile on the plane 7)loop to step 3

Our SolidSketch add-in

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has a "Sketch Sweep" feature which can do the job from your 3D Sketch. Next version will do it directly from edges, unless 2005 does it to... If not, fill an enhancement request ;-)

Reply to
Philippe Guglielmetti

Here's another approach..

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..

tomcrick wrote:

Reply to
Paul Salvador

and a very good idea it was too!

Reply to
neil

Thanks Paul!

That is much appreciated ? you have saved me countless hours of fiddling! Actually, I was just about to sit down and have a play with surfaces. I really need to become more familiar with their use in Solidworks but I don't get time to play much as I usually work with ProE and UG.

Today it really struck me just how useful the internet can be!

Cheers

Tom

P.S.

Thanks also to Philippe for his composite curve trick. I'll use that method with some of my sweeps in the future.

Reply to
tomcrick

Paul made some suitable surfaces: to match the plan view , an outside offset of the plan view, and a side profile of the top, and offset a surface below that one, and mutually trimmed to end up with a L shape ,applied a suitable draft and thickened to a solid. This is a much neater solution than sweeping for this particular example. If you are interested Andrew I will send you a few small screen shots by email. cheers neil

Reply to
neil

Reply to
Paul Salvador

Neil and Paul

A nice example of how the 'obvious' approach is often not the simplest or best. I think humans should be equipped with a klaxon which goes "aa-oo-ga" repeatedly whenever we start shooting from the proverbial hip, prematurely uttering those fatal words (to paraphrase Clark Kent) "this looks like a job for super-sweep !", or whatever other 'tool du jour'.

Thanks, both of you. This ng rocks!

Reply to
Andrew Troup

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