After posting last weeks example of Using Guide Curves in a Sweep, I received a comment and an email with two very good suggestions.
The first was a comment asking if I could have simply used a Full Round Fillet and achieved the same result. I had thought about trying that method when creating the model but I didn't think it would work because of the change of the face in height as it went around the part. So here is a shot at doing it that way:
As you can see as the fillet travels up to the different elevations it doesn't follow the change and produces an unwanted result. Good suggestion, but unfortunately it wont work for me this time.
The second message I received was from fellow SolidWorks Employee Mark Biasotti explaining some of the benefits of using surfaces to create the same feature, namely that it rebuilds much faster, and he also pointed out that I could have saved time by using a command available in the sweep command.
In the previous blog post I mentioned creating two separate 3D sketches to use as guide curves. Well lets see what Mark suggests we do.
In the feature manager of the sweep command if you right click in the guide curves box, you get the selection manager tool as an option:
After using the Selection Manager to select a group of edges, I now ended up with this result:
Now the two guide curves are created inside the sweep command without the need of having to create two separate 3D sketches.
Here is a hint when you use the Selection Manager tool and use the Select Group option:
Once you click one edge, click the tangency option that will pop up (highlighted in red in the picture below) and that will select the tangent edges of that edge and you wont have to click all the edges:
The result is the same part but with less work, and less features. Thanks for the comments and suggestions!