20 people attended this meeting.

Click on links for easy navigation

1. Create reference planes and points in space to define the profile path. Point visibility will need to be turned on.
   
2. Select Curve Through Reference Points and select the points in order. You can find this command from the Curves drop down icon, shown, or you can select it from the Curve menu under Insert.
   
3. Sketch the desired profile on a surface at one of the end points of the curve.
   
4. Select the Swept Boss icon. Choose the profile sketch and the swept curve for the Profile and Path.

As was demonstrated, if the curve makes too tight of a bend for the sketched profile, you will get an error message to that effect.

You will usually want to select Maintain Tangency in order to get the effect that you want. In order to get the desired effect, you will likely want to start with two points one at the starting surface and normal to your starting surface and a small distance out.

You can easily change the swept path by moving the points.

This technique will be effective for tube routing.

Teams were chosen based on grouping people with different backgrounds. No two people could be from the same company. Fortunately, we also were able to mix people with diverse SolidWorks experience.

The part that was to be modeled was a three-part weldment with machined features. We identified these different ways to model the part.

• Model the individual weldment parts (bottom up) and combine them in an assembly file. Remove material in the assembly to reflect the machining operations.
  
• Model the weldment parts in place in the assembly (top down). Remove material in machining operations in the assembly.
  
• In an individual part drawing, model all of the welded components. Either merge the parts or not. Add the machining features in a separate configuration.

There are variations on these themes and other ways to approach the model. One variation joined the assembled welded components into a single part and then machined that part. Details on how to join the parts can be found in the May 22, 2003 NEWSUG meeting minutes.

The discussion about selecting modeling approach fell along the lines of modeling parts to match the bill of material structure and modeling parts to match the manufacturing steps. One suggestion was that we should model along functional requirements and look at manufacturing steps only when we are indifferent about the functional requirements.

• In deciding to put fillets and radii on a flame cut part, best practices usually recommend that we add them in a subsequent step to the general layout. In practice, many of us prefer to put everything in one layout.
  
  Putting everything in a large layout saves an insignificant amount of file space. It keeps the SolidWorks FeatureManager Design Tree short. When the part is simple or has only medium complexity, the Design Tree might have only a few entries so that there can only be a few wrong places to look and finding things can be efficient.
  
  As parts become complex, the logic of putting everything in a few complicated sketches breaks down and the generally recommended practice will be a better solution. This approach makes labeling the features a more compelling requirement.
  
• Few of us are disciplined enough to give the features in the FeatureManager Design Tree unique names. We get away with this when the number of entries is modest and revisions are made recently. Proper labeling will be essential as the models become large and they are moved from worker to worker.
  
• When the model is simple and the designer modifies his own model shortly after he made it, he can get away with bad practices.

One of the challenges of the model was sketching a flame cut joggle in a profile. The joggle was offset by 12 mm and it was joined by tangent 10 mm radii. The joggle was located from an edge with a dimension to a radius tangent point. The most efficient way to create the general geometry is to sketch the approaching line by clicking on the line end points. Then click on the end points of the two arcs and the exiting line. When clicking on the end points like this, you can toggle between line and tangent arc in either of these ways:

• Select the letter a from the keyboard to toggle between line and arc.
  
• After you click to end a line and move the mouse away from the line end point, move the cursor over the line end point again. This works only to convert the cursor from a line to an arc and not toggle from an arc back to a line.

Extending the functionality of the Sketch Trim tool

In the process of exploring other options, we learned that the Sketch Trim tool can be used to extend a sketch line.

• With the Sketch Trim tool selected, click on the line that you want to extend and drag it to the line that you want to extend it to. When the line visually extends, release the mouse button.
  
• With the Sketch Trim tool selected, right click and select the Extend Entities command from the drop down menu. This is a toggle option that will let you go between Sketch Trim and Extend Entities.