Consumer Product Design with SolidWorks

Michael LaFleche — Wed, 03 Mar 2010 15:13:20 +0000

Many times, an industrial product designer will sketch out the design either on paper or on software like Adobe Illustrator. These designs are very stylized and a lot of thought is put into these drawings. Wouldn’t it be nice if you could use these designs more readily? SolidWorks has all the tools available for this process. In the first part of the demonstration that I am giving, I will insert a picture into my SolidWorks model and use that as the basis for a new design. Since I have a lot to show in the webcast I will not have to to show the following steps in detail, so here you go! Let’s work on a remote control design. Step 1 is to take a digital format drawing into SolidWorks. We support many raster formats, but we will bring in an Adobe Illustrator file as shown in image “A” below. The next step is to format the picture so that it lies on top of the origin of the SolidWorks model, so we can take advantage of the datum planes we already have. Simply zoom in and drag the sketch to position it. A little known feature that SolidWorks has in the Add-Ins list is the “Autotrace” tool. (See image “B” below) This allows you to actually convert the raster image to vector information if you have a crisp and clean image. Chances are you do not have this tool turned on, but is is part of every seat of SolidWorks since 2008 I reckon. If you have this Add-In turned on, you will have an arrow in the PropertyManager for the Sketch Picture command as shown in image “C”. Now that the tool is available, you can edit the sketch picture with the sketch that you have inserted it into open, by double clicking the sketch on-screen. Then the arrow is available and you can use the tracing tools that SolidWorks has now revealed. Choose a selection tool, like a rectangle or a lasso, and select what you want to convert on the screen. In image “D”, I used the rectangle tool to select the end of the remote control. If the entities do not look too good using your picture, then you can play with the “Adjustments” settings inside the PropertyManager. Very often changing the brightness and image contract will make your sketch conversion look smoother.

Of course, this is only one way of using imported data, and very often you will find manually drawing lines and splines will do a better job as you can assign parametric behaviors to those elements in an easy way. Then there is the who other topic of importing 3d scan data, which I plan on getting to at some point. Make sure to check out the webcast Thursday by clicking here to sign up. It is better if you can watch live as it is interactive and you can ask questions. I will of course record it and edit this post with a link to the recording.

To Derive or not to Derive, that is the question…

Michael LaFleche — Mon, 01 Mar 2010 21:25:42 +0000

One of our Application Engineers pointed put a often overlooked function in SolidWorks called “Derived Sketch”. This tool derives a sketch from another sketch that belongs to the same part, or derives a sketch from another sketch in the same assembly! When you derive a sketch from an existing sketch, you are assured that the two sketches will retain the characteristics that they share in common. Changes that you make to the original sketch are reflected in the derived sketch. To derive a sketch from a sketch in the same part: Select the sketch from which you want to derive a new sketch. Hold the Ctrl key and click the face or plane on which you want to place the new sketch. In the example below, I created an Offset Reference Plane by holding the CTRL key and dragging one of my planes away at 1 inch. Then I chose Insert, Derived Sketch from the pull-down menu. This is one of those secret handshakes in SolidWorks where you have to pre-select to get the command to appear. (It is a species nearing extinction, now that “Convert Entities” now has a property manager interface in SolidWorks 2010. Now that you have initiated the secret handshake, the sketch appears on the plane of the selected face, and the status line indicates that you are editing the sketch. Position the derived sketch by dragging and dimensioning it to the selected face. (The derived sketch is rigid and drags as a whole entity.) I rotated my sketch 90 degrees about the midpoint of the first sketch. You can add relations to the original sketch so that things are coincident, parallel, ect… Then exit the Sketch. Make a feature like normal. In my example I created a lofted feature. Now if you change anything in the original sketch, the other sketch updates.

If you wish to “un-derive” the sketch so that it no longer receives the updates of the original, simply right-click the derived sketch feature in the tree and choose Un-Derive. Thanks to Paul Hagenow of CAPINC Technical Support for suggesting to post this topic!

CAPUniversity » Sketch

Consumer Product Design with SolidWorks

To Derive or not to Derive, that is the question…