Help with sweeping lip along 3D sketch?

Question

Hi,I'm having problems sweeping a lip along a 3D sketch created from theedge of a part I am modelling. Although it looks a pretty simple thingto achieve I can't seem to get it to merge fully with the part andhave tried loads of different methods.I've posted some screen caps and the part file at the followingaddress instead of trying to explain it all in words. 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

Philippe Guglielmetti · Accepted Answer

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 ;-)

Paul Salvador · Answer

Here's another approach..tomcrick wrote:

neil · Answer

and a very good idea it was too!

tomcrick · Answer

Thanks Paul!That is much appreciated ? you have saved me countless hours offiddling! Actually, I was just about to sit down and have a play withsurfaces. I really need to become more familiar with their use inSolidworks but I don't get time to play much as I usually work withProE and UG.Today it really struck me just how useful the internet can be!CheersTomP.S.Thanks also to Philippe for his composite curve trick. I'll use thatmethod with some of my sweeps in the future.

neil · Answer

Paul made some suitable surfaces: to match the plan view , an outside offsetof the plan view, and a side profile of the top, and offset a surface belowthat one, and mutually trimmed to end up with a L shape ,applied a suitabledraft 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 byemail.cheersneil

Paul Salvador · Answer

Thanks, Neil!neil wrote:

Andrew Troup · Answer

Neil and PaulA nice example of how the 'obvious' approach is often not the simplest orbest. I think humans should be equipped with a klaxon which goes "aa-oo-ga"repeatedly whenever we start shooting from the proverbial hip, prematurelyuttering those fatal words (to paraphrase Clark Kent) "this looks like a jobfor super-sweep !", or whatever other 'tool du jour'.Thanks, both of you. This ng rocks!

Help with sweeping lip along 3D sketch?

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