CAPINC Technical Blog

Central MA and Northern CT SolidWorks Users Group on March 10th

Michael LaFleche — Wed, 10 Mar 2010 18:36:17 +0000

The Central Massachusetts and Northern Connecticut SolidWorks Users Group (CMNC-SWUG) will be meeting tonight at Metso Automation at 44 Bowditch Drive, Shrewsbury MA, 01545. The festivities begin at 5:30pm with networking and refreshments. The presentations for tonight’s meeting will be delivered by Tom Cote, of Veeco Solar Equipment and Bruce Holway, of Dassault Systemes SolidWorks Corporation. Tom will present SolidWorks Configurations and Design Tables and Bruce will talk about the Weldment tools in SolidWorks. To sign up for this free event, click here. I hope to see you all there…

“Big” News for SolidWorks Users

Keith Pedersen — Wed, 10 Mar 2010 14:30:02 +0000

In doing some investigation relating to the actual dimensional limits of SolidWorks CAD models I came to some compelling conclusions. Solidworks models are dimensional, (rather than unit-less) and the native modeling basis is 1 meter. The largest possible model dimension is 1000 meters, (39370.07874016 inches) and the smallest possible model dimension is 0.00001 meters, (0.00000394 inches). To put that in perspective, that is the size of 1 human red blood cell. In theory you should be able to fit a part file within a 1km x 1km x 1km cube. In practice, the best reliability (especially with graphics) comes from limiting a part model to +/- 350m. Because circles are stored via their Diameter value, not via Radius, arcs are actually limited to a 500m radius. Note – assembly files extend your working envelope. For example, If you model a city block as a part file 1 km on a side, you can lay out a ‘city’ of many of these blocks in each direction. Mates will still work, measurements and dimensions will report accurately, up to a working limit of 100km x 100km.

Design Cams in SolidWorks

Michael LaFleche — Mon, 08 Mar 2010 21:45:12 +0000

Did you know that you can create cams with fully-defined motion paths and follower types with SolidWorks if you have the Toolbox Add-In turned on? You can choose circular or linear cams with many motion types. You can select the follower track as a blind cut or cut through the entire cam. To create a Cam, Click Cams (Toolbox toolbar) or in the pull-down menus click Toolbox > Cams.
In the Cam dialog box, on the Setup tab, for Cam Type, select Circular or Linear and set property values for the cam type you selected. See images below. You can also create a cam based on a previously saved favorite cam. I recommend starting off with this so you can see how the cam is created. Once you have the jist of how the cam is created, venture out on your own be creating a new one based on your specifications. SolidWorks has a lot of great information on building the cam on their new web based help system. Check out this link showing how to create the cam motion here. Below are images of some of the Cam tool option tabs.

Once you create your cam, you may discover it looks a little rough. This is because by default it creates the cam in arc segments one by one. If you want it to be even rougher, you can un-check the “arc” option in the cam generation tab to have it generate line segments. For a smooth surface, you can convert the line segments or arc segments to a spline. To achieve this, edit the sketch of the cut that generates the cam path, then select the entire path of the cam and go to Tools > Spline Tools > Fit Spline. Here you should select that you want to contain the spline to the original geometry plus convert the original geometry to construction lines. See the images above for a comparison of the different options for generating a cam.

SolidWorks Enhanced Interrogation Techniques: Part II

Michael LaFleche — Thu, 04 Mar 2010 20:08:36 +0000

Assembly Visualization provides different ways to display and sort an assembly’s components in a list and in the graphics area. You can sort the list by one property at a time. Basic calculated numerical data such as component mass, density, and volume are available in the tool. Additionally, you can create customized criteria which are dependent on several numerical values! If you defined noncalculated properties such as Vendor or Status in the component files, you can access those properties for modification and sorting. Properties from SolidWorks Sustainability are also available.

Here is a quick tip to help you find parts & sub-assemblies, within an assembly, that have long rebuild times. Using the Assembly Visualization tool in SW2010, you can sort all the components of an assembly using their Rebuild Time as the sorting property. See the link to a movie showing this here. SolidWorks Assembly Visualization Video

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.

Boston Area SolidWorks Users Group on March 4th

Michael LaFleche — Tue, 02 Mar 2010 15:36:34 +0000

On Thursday, March 4th the Boston Area SolidWorks User Group will be meeting at American Science & Engineering Inc at 829 Middlesex Turnpike, Billerica, MA 01821. The agenda starts off at 5:30pm with networking with other SolidWorks users. Food and refreshments will be available. From 6:00-6:15pm Opening statement from BASWUG Committee and from 6:15-7:30pm Keith Pedersen our Principal Applications Engineer at CAPINC will present one of his SolidWorks World 2010 presentations entitled: Beyond the Weldments Toolbar. This presentation will briefly review the underpinnings of the Weldments functionality in terms of multi-body solids. To signup, click here….

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!

SolidWorks DXF Output for 2010 – for Sheet Metal parts

Michael LaFleche — Fri, 26 Feb 2010 19:47:57 +0000

This is the second blog post in my manufacturing series. This scenario of outputting parts to DXF format for laser, waterjet, punching and so on should be used for parts with sheet metal bends. When creating parts using the Sheet Metal functions, SolidWorks will calculate the flat pattern. New in SolidWorks 2010, users have the capability of automatically creating a DXF file without creating a detail drawing and exporting from there. This snuck into SolidWorks 2009 if you had a sheet metal part as well, but it was not as robust as the 2010 method. In 2009, you need to have a sheet metal feature in your part and then you would go top the File… Save As… Menu and choose DXF or DWG. Then you would go ahead and clean it up by removing the bend lines and any other geometry in DWGEditor, so as not to confuse the CNC software. In SolidWorks 2010, the solution is much more elegant. Follow the gallery below for a full description of how this works, but essentially, you can right-click on the “Flat-Pattern” feature in your FeatureManager Design Tree, then choose “Export to DWG/DXF” Then it will ask for a file name. You will then be presented with a PropertyManager that shows a Sheet Metal radio button as the default choice. Then you can decide if you just want the geometry “Arrow A” or if you want to include the Bend Lines “Arrow B” You would use automatic bend line if you have automated bending equipment and your CNC software can interpret it. Save out he file and you are all set!
Another nice thing in 2010 is the quick toggle for a flat pattern. Especially in the light that you can have more than one flat pattern for a sheet metal fabrication. Right-Click on any sheet metal body in your design and you can choose “Toggle Flat Display”. Here you will see a preview of the flat pattern on your screen available until you move on to the next command.

SolidWorks DXF Output for 2010 – for Waterjet, Laser, ect…

Michael LaFleche — Thu, 25 Feb 2010 21:52:02 +0000

In working with several customers and preparing for my webcast on SolidWorks for Aerospace Component Manufacturers (watch recording here), I realized how powerful the new DXF/DWG output capabilities in SolidWorks 2010 were. Simply put, a manufacturing engineer can output a DXF file from a SolidWorks model without the need to make a detail drawing. This is handy if you are going to the waterjet, flamecutter or laser with a 2D profile. In this article, I plan on showing you methods for exporting to DXF when you have different manufacturing scenarios.

The first scenario is a part that needs to be flamecut or laser cut and does not need to be bent on a press. Step 1: Right click on the face you wish to create 2D DXF output for and choose “Export to DXF/DWG”, choose a filename. Step 2: Modify the options so that the origin is in the right place for the laser software if you wish and choose “OK”. Step 3: Preview the DXF output image. You may remove unwanted geometry, such as fillet radii or hidden lines and choose “Save”.

In my next blog entry I will show you how to export Sheet Metal parts that need to be bent.

SolidWorks Enhanced Interrogation Techniques

Michael LaFleche — Tue, 23 Feb 2010 20:41:40 +0000

SolidWorks provides ways for you to get your assembly models to talk. You don’t even need to bring in Jack Bauer (a shameless and gratuitous “24″ plug). You will find that the SolidWorks AssemblyXpert will come to the rescue when your model is either behaving badly or not at all.

The most common use for the AssemblyXpert in SolidWorks is to ask the assembly how many parts it has. No need for Sodium Pentathol here. Just go to the Tools… pulldown menu or the Evaluate tab in the Command Manager and choose AssemblyXpert. You will then be presented with a host of stats relating to your design.
You will note it spills it’s guts relating to top level components, mates being solved, ect…

I got a great tip from my colleague at CAPINC Al Zullo while he was working with a customer. The customer’s assembly disappeared, all the components in the feature tree were still showing. The zoom to fit command blew the screen to infinity. Once again, we bring in the AssemblyXpert. The tool told us that there was a component “very far away from the origin” and showed a wrench button….click….moved the component into view and the zoom factor fixed itself. He didn’t even need to initiate waterboarding!