Newbie: Surface Blend Question?

[sbird]

Dear All
I am a tech/tutor at an English design college, learning and teaching Solidworks (basic level)


If any could help with a technical question regarding Surface modelling I would like to ask:

when teaching Rhino3D (to create a teapot for instance)
a 'intersection' curve is created between eg. spout and main body
then turned into a pipe shape to cut into both surfaces
These cut surfaces are then joined by using 'blend surface' rather than fillet.
This an extremely useful and much used technique in our department.

I am trying to fnd a similar technique in SolidWorks but have had no luck.
I would be grateful for any advice you may have in this area.

Many Thanks

Simon Bird

Technician/Tutor
Royal College of Art
London
UK

 

[staabe]

Simon,
I'm relatively new also and have ran into the same issues. From what I have experienced the only way to do this is by trimming the surfaces, thickening them to form a solid and then using a fillet for the blend (assuming you're using SW '05 or '06.)
I believe now in SW '07, SW has added that blend feature along with a few other more advanced surfacing techniques.
As stated, I'm new so there very well may be a way to do it but I have not figured it out either.
Good Luck!!

 

[bcampbell]

I typically never solidify my model until I'm done with the shape. Organic shapes are simplier using surfaces, ribs and bosses are more easily done in solids.

Parametric surface modeling, solidworks can create a surface model that's parametric. This will allow changes to the initial surfaces and allow you to rebuild everything to accept this change. This to me should be a requirement for any design tool.

Anyway, sorry, I was in sales at one time.

Curves in solidworks can be created by a sketch plane or by a surface to surface intersect. There's an icon that's not displayed in a standard install which ca be added to your sketch tool bar. This icon when selected will:

1. if in a 2D sketch, create a 2d curve between the sketch plane and any choosen surface that intersects with the sketch plane.

2. if in a 3D sketch, create a 3d curve at the intesection between 2 surfaces.

Now you can do what ever you want with these curves.

The blending in solidworks is handled mainly in the loft function. The options found here fulfill most of my blending needs. Here you can define a loft between 2 curves or 2 surface edges. If you use 2 surface edges, you can take advantage of the 2nd order blending (curvature continous) associated with the edge and it's related surface. Please keep in mind that a 3D curve in space doesn't have a surface associated with it and therefore, 2nd order blending is difficult due to fact that there is no direction coming off the curve. Sometimes solidworks figures out the curve to surface relationships sometimes not. It depends on the release. Play it save, if your planning on tangential or 2nd order blending, use a surface edge as opposed to a 3D curve.

You can visit our techtip area, search on surfaces.

http://66.89.101.227/web6/tips.html?name_picked=surface_intersections&search=surface

 

[bcampbell]

Solidworks 2007 has a new push/pull capability that allows you the ability to tug on existing surfaces without creating construction curves. This will greatly simplify the ability to add a pimple on a surface if that's what you want.

More extensive changes can be made to a surface by broadening the scope of the deformation shadow. What's really cool is how solidworks handles the edge conditions once a surface has been tweaked. It snap the deformed edge back to the original edge so that your 3D manifold is still valid.

This is really cool, if you haven't seen it, you need to attend a 2007 rollout and watch this this new functionality.

 

[sbird]

Many Thanks for both your replies.

Bill: the Intersection curve tool is just what I have been looking for, once I understood it.

I'll try the convert entitys next.

Just after writing the email I tried projecting a circle curve on 'teapot' surface, sweeping (pipe)it then using it to trim
cutting both spout and body, then creating a fill between them, then apply knit, then thicken. It looked ok...

Thanks again

Simon

 

[PipSqueak]

Simon
I am setting up a London based SolidWorks user group SWUG (with the support of the SolidWorks user group coordinator)
the first get together is planned for 12th Oct @18.30 in Hammersmith
if you are interested then contact me

Regards

Nick Ford
[email protected]