boundary surface in SW

When I create a surface boundary with as series of curves forming a four part boundary two of which are the same 3d curve, how can I get solidworks to refrain from consuming those curves once the surface is bundled into Boundary-Surface.

When you say “consuming”, what do you mean? You should still see the curve, it’s just hidden, right? It’s embedded into the feature the same way Pro/E does.


Yeah, it also hides the curve but you can show it again, as well as reuse it for other features where it becomes a shared sketch.

There must be a configure setting someplace.

Possibly… but I doubt it. The only features I can think of that don’t hide sketches are Weldments for whatever reason.

If you expand the Surface feature in the tree, it should have the curves listed below it. Just right click and hit “show”. Also make sure that your curves are toggled to visible. You can toggle this through the selection filter.

By consumed, you mean when SW says “these curves/sketches are being used by another feature”, right?

Sometimes I make a second set of curves, using ‘use edge’ so that the first set aren’t consumed.

Good point. Yes, I’ve seen that before and using the edge to make duplicates is the way to go.


Hm I don’t think I’ve ever encountered that. But a duplicate sketch is good when you know it’s something you’re going to be tweaking back and forth, esp using Instant3D.

What bothers me is that sometimes you can end up by having the sketch filed behind another feature that is referenced to that very sketch. You can trail back by rolling back the features but not the sketches, but I would like to see an option of a sequential feature tree, including sketches. In fact, I did contact my VAR about it, and they assured me it wasn’t possible.

How can I change one curve segment to one color and the other curve segment to a separate color? And how can I place mesh lines onto a surface w/o editing the feature.

:confused: Now you talking crazy. Never done it.

okay… this one may be a little crazy talk too. Building a surface boundary to two trimmed surfaces. One side looks at the surface edge while the other side looks at a projected curves (surface edge under there). I can get tangency on the one side but since the second side looks at the projected curve I cant get tangency… unless I look instead at the surface edge. How can I get tangency to the surface edge even if I want to look at the curve?

You can right-click on a sketch or curve and use Sketch Colour or Curve Colour. This will only pick entire sketches or curves though, so, no selection of individual entities like the SelectionManager allows you in a Boundary or Loft.

You can place mesh lines by selecting the surface and using Tools - Sketch Tools - Face Curves. You can set the amount of UV lines you want to see and generate 3D Sketches for each one if you want to use them for another feature.

Are you projecting your sketches that you wish to trim with, using Tools - Curve - Projected unto the surface and then trimming with that curve? That is not necessary in Solidworks, if your sketch lies on a plane you can use Insert - Surface - Trim and select your sketch you wish to trim with, it will project the sketch automatically along the plane normal and allow you to trim, right there.

In general. Curves in Solidworks are (and excuse me if I am mistaking) more of a remnant of the past, when thing like the SelectionManager wasn’t there and all that, as a way to reduce multiple sketches for lofting this, and that. These days it’s just a lot easier and Curves are somewhat obsolete for most purposes.

Curves can not be shared.
Curves have lower accuracy in some cases.
Curves have no defined plane so can not use normal to profile with lofts or boundaries.

Sketches are where it is at! :slight_smile: