Mike Puckett's Blog

Using Guide Curves in a Sweep Part 2

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!

Using Guide Curves in a Sweep

While recently creating a model for an upcoming Certification exam, I ran across the use of a function that may or may not be widely used when creating sweeps in SolidWorks.

The part I'm creating calls for a wavy design that has a round feature that sweeps along its outside path:

 

Here is the side profile:

 

I started off with a square shape that has the wave built in it:

 

Then it was a matter of cutting the circle out that I wanted:

 

Now is where the sweep with guide curves comes in.  Step one is to create the profile that will get swept along the outside of the part:

 

The next step it to create the path that the profile will follow.  To do this I started a 3D Sketch, right clicked on of the edges, then selected "Select Tangency":

 

Normally this is all the information you need to create a basic sweep.  The issue with this example arises because the sweep is going to be changing elevation along the path, so guide curves will be necessary to tie it down.  Let's look at how the sweep would preview if I used the profile, and path already created:

 

The preview looks ok from the front, but along the back of the part is where there are issues:

 

You can see how the profile is not staying along the face as it changes elevation.  In fact this sweep fails if you try to accept it.  The solution was to add not one, but two guide curves to keep the profile traveling along the correct path.

On the options tab, you can select the "Follow 1st and 2nd guide curves" from the pull down: 

At this point you will have to have two additional 3D sketches already created.  Using the same selection of the tangent edges as shown above, you would create two 3D sketches that would like like this:

  

They must be in separate sketches, and you will not be able to select the path as a guide curve in the sweep manager.  You will end up with a preview like this:

 

Upon successful completion, you will have the part looking just as I have mine:

 

Just about every SolidWorks feature has multiple options to help make a model come out the way you need it to.  By exploring these options, chances are you will get what your looking for without the need for additional features or steps.

By the way, this model is going to be used in an upcoming exam that will have the user create a mold parting line.  Here is a look at the final part:

SolidWorks Set To Launch Engineering Stimulus Package

On Monday April 6th, 2009 SolidWorks in partnership with over two dozen North American SolidWorks Resellers will officially launch the 'SolidWorks Engineering Stimulus Package' program to out of work engineers in the United States and Canada.

The Package includes:

• A free down-loadable 90 day version of the SolidWorks Student Design Kit including eDrawings
• Online documentation
• Access to Solid Professor training materials
• And a free shot at achieving the Certified SolidWorks Associate certification (CSWA)

Those VAR's participating in the program will also offer additional training materials and services at their discretion.

The program is meant to aid out of work engineers in keeping their SolidWorks skills up to par while they seek new employment, and also to help give non-SolidWorks engineers a good understanding of SolidWorks to help them also achieve a new position.

More information about the program including a special video message from SolidWorks C.E.O. Jeff Ray can be found at the Engineering Stimulus Package website via this LINK.