This blog is Part 4 of a multi-part blog and video series examining the difference of creating a simple bookcase using Top-Down Assembly modeling and Multi-body Part Design techniques. In this blog, we will examine the methods used to create Library Feature Parts and Smart Components used for both.
SolidWorks makes it possible to create a library of geometry that can be used over and over again without having to recreate it from scratch each time. This is accomplished by employing the use of the Design Library. The Design Library is accessed on the Task Pane and can contain a wide variety of data including features, parts, assemblies, forming tools, annotations and many other types of cad data. When SolidWorks is first installed, it provides a starting point with some basic samples of reusable CAD data organized into a basic folder structure. The intent for this is to serve as an example for the user to start with in order to create their own library. It is recommended that the user should set up a folder structure that can be managed outside of the standard SolidWorks installation directories to define a custom Design Library. The image below shows the Design Library tab active on the Task Pane. Notice the buttons at the top of the image (with the colored arrows pointing to them). Refer to the explanations for each in the key at right.
For this example, I created the MY DESIGN LIBRARY folder on my local C:\ drive using Microsoft Windows Explorer. I then used Add File Location to add the new folder to the Design Library. Next, I used Create New Folder to create a folder inside the MY DESIGN LIBRARY file location called Furniture. It is here where I will place the Adjustable Shelf Holes Library Feature Part that I can reuse in my designs. In order to create the Library Feature Part, it is necessary to create a defining part for the features I need.
The image to the right illustrates the defining part that holds the hole and pattern feature needed for the Library Feature part. Notice the part is a very simple part with three basic features:
- A Boss-Extrude that represents a basic panel. This base feature will NOT be included when the Library Feature Part is created.
- A simple cut representing the lower 2 holes, or the seed, of the adjustable hole pattern. The dimensions of the sketch of the holes is indicated in the image. The depth of the hole is 0.25in. This feature WILL be included when the Library Feature part is created.
- A simple linear pattern feature to complete the hole pattern. Instance count is 4 and spacing is 1.00in. This feature WILL be included when the Library Feature part is created.
Once the defining part with the desired features for the Library Feature Part is created, it is time to use the Add To Library command at the top of the Design Library. While the defining part file is active and the Add to Library command is activated, the user is presented with a property manager as illustrated in the image below. At the top of the Property Manager is a blue selection box. For this example, the Cut-Extrude1 and the LPattern1 features are selected from the Feature Manager Tree flyout in the graphics area. Below that is a text field box to assign a File Name to Save To, in which Adjustable Shelf Holes is typed in. Notice the Furniture folder created earlier is selected from the Design Library folder selection box. Once selected, it is also highlighted in the MY DESIGN LIBRARY folder in the Task Pane at right. At the bottom of the property manager are options for adding a description and selecting a file type. For this example we will make sure that Library Feature Part is the file type selected.
Once the property manager is properly filled out, select the green check to accept the parameters and finish the command. The Library Feature Part is created and added to the folder defined in the Property Manager. This results in a file called Adjustable Shelf Holes.sldlfp saved into the Furniture folder created previously. When the Design Library folder is selected in the upper portion of the Task Pane, the contents of the folder will be displayed in the lower pane. At this point, the defining part is no longer needed. It can be saved if desired, but really has no value any longer as the Library Feature part is created in its own file. There are no file references linking the two files together. There are some edits that could be made in the newly created Library Feature Part, however. Double clicking the file in the lower pane will open it in its own window and further edits to the file can be realized.
Refer to the image below. For this example, I have opened the Adjustable Shelf Holes.sldlfp file and renamed some of the dimensions. Examination of the Feature Manager Tree on the left reveals some characteristics that have been created in the Library Feature Part. At the top of the Feature Manager Tree a few folders and sub-folders have been added. These have been expanded to reveal the contents. The folders contain information that will control how the Library Feature Part will behave when being used in a design. The first folder is References. These are the items that SolidWorks will use when placing and orienting the Library Feature Part in a design. The Dimensions folder is used to organize dimensions from the Library Feature Part that can be; 1) overridden during placement (these are the dimensions with names to them in the Dimensions folder), 2) used for locating the feature (placed in the Locating Dimensions sub-folder and used for locating the feature when placed. No locating dimensions are needed for this example), and 3) for dimensions that are to be kept internal to the Library Feature (dimensions not needed for overriding size or used for locating the feature). Dimensions are renamed, and then, using a drag-and-drop process, can be reorganized into the appropriate folders. Notice the Cut-Extrude1 and the LPattern1 features at the bottom of the tree have an “L” icon superimposed on them. This indicates that these are the actual Library Features that will be placed in the new design. The Boss-Extrude1 feature is the minimum geometry needed to create the library features and will not be transferred to the new design. Once the organization of the dimensions is complete, the file is then saved and closed and is now ready to be used in a new design. More information on creating Library Feature Parts are addressed in some of our advanced classes.
Now that the custom library has been created and the Library Feature Part is defined and saved into the Library, it can be used in the new bookcase design. Using the Library Feature Part is the same for both versions of the bookcase, Top-Down Assembly or Multi-Body Part. In the case of the Assembly, open one of the side panel components in its own window and place the Library Feature Part. For the Multi-body Part Design version, the Library Feature part is placed on the individual side panel bodies. Using Isolate can be helpful when working with multi-body parts.
Refer to the image below. Using Library Feature Parts from the Design Library is a simple drag-and-drop process. Choose the appropriate folder from the upper pane of the Design Library, select the file from the lower pane, and drag-and-drop the file onto the face of the part in the graphics window that will receive the features. This action will open a property manager for the Library Feature Part and place a preview window of it in the graphics area. The preview window serves as a key or guide for choosing the correct Reference needed to place the features. The property manager of the Library Feature Part takes the information from the folders that were added to the Feature Manager Tree of the Library Feature Part when it was created and places the information in the appropriate group boxes of the property manager. The References folder of the Library Feature Part contained a Placement Plane and two edges. The face that the library feature part is drag-and-dropped onto is placed in the Placement Plane field of the property manager. The other two references are the edges that the original features are dimensioned to in the defining part file. Referring to the image below, the Preview in the graphics area is highlighting one of the edges. This indicates the corresponding edge that should be selected in the destination part. As the edges are selected in the destination part, a green check will appear next to the edges listed in the References selection box of the property manager. Initially, the references listed in the box will have a question mark next to them, (as can be seen in the image below), until a selection is made in the destination part. Once the References have been satisfied the preview window will disappear. Any locating dimensions that were dragged into the Dimensions\Locating Dimensions folder in the Library Feature Part will be listed in the Locating Dimensions group box of the property manager (there were none for this example). Any dimensions that do not get organized into the Locating Dimensions or Internal Dimensions sub-folders and remain in the Dimensions folder, (all of the named dimensions in this example), are placed in the bottom group box of the Property Manager titled Size Dimensions. The dimensions are activated by placing a check in the box titled Override Dimension Values. Once the references are satisfied and dimensions are modified if necessary, selecting the green check will end the command and the library feature is added to the bottom of the Feature Manager Tree of the destination file.
Once the Library Feature of the Adjustable Shelf Holes is added to the bookcase design, configurations can be defined for the design. The result is a very flexible system of shelves that represent the sizes in our office that I now can use in the office model.
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