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.

http://tom.jahingoonline.co.uk/downright/solidworks.htm

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

 

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 (www.solidplus.com) 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 ;-)

 

Here's another approach..

http://zxys.com/misc/LipHelp-zxys.zip

...

 

and a very good idea it was too!

 

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.

 

For those of us longtime supporters of SolidWorks who're registering a
protest about declining reliability standards by boycotting subscription
(tugs at the heartstrings, don't it!) and consequently get the 'future
version' message when trying to open example models:
Can anybody still on the upgrade treadmill briefly interrupt their trudging
to describe Paul's solution?

(Assuming it lends itself to a brief description, otherwise I'll put it down
to one of the prices I pay for allowing a stubborn nature free reign)

 

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

 

Thanks, Neil!

 

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!