Here we are at the beginning of another fine week in the blogosphere. I hope each and every one of you had a great weekend. I also hope you got some rest because I have tons of tips and tricks to throw your way this week. Today we will start with our continuing exploration of the benefits of using the Design Library. In the past we explored such topics as creating a notes library, adding forming tools and adding components to the library with Mate references. If you missed any of these post you can go here to find them all: http://www.theswgeek.com/tag/design-library/. Today we are going to cover adding your most commonly used features to the design library to speed up your design process.

Prepping Features to be Added to Library

You might recognize the plate below from last week’s discussion on adding items with mate references. The plate has the hole pattern required for use with the linear bearings and this hole pattern is used often. Rather then create the hole pattern every time we need to use a linear bearing, we can add the pattern to the Design Library to be used on future designs.

First, we need to make sure that our sketch is set up properly prior to adding the features to the Design Library. There are a few things you may notice about the sketch shown below, the first being that the sketch is not fully defined. I do not have the location of the feature specified, this allows me to define the location when inserting the feature into other parts. If you find it desirable to have the feature be located in the same place in future designs, add locating dimensions at this point. The next thing you may notice is that I have a point at each quadrant of the outside construction circle. I use this technique to control the location of the threaded holes in the next feature with one diameter dimension.

Next, since there are a number of sizes of available for linear bearings, we want to have the hole pattern dimensions change per size of bearing. Right-click one of the dimensions and select Configure Dimension from the menu.

In the Modify Configurations window add the required part configurations and enter the appropriate dimension value. Do this for each dimension that will change in each configuration. Once all the dimensions are update exit the sketch.

Find Appropriate Folder for Features

Every user may have a different folder structure for the Design Library, so it is an individual choice as to which folder you will save features. Dig through your Design Library structure to find which folder you would like to add the feature.

If your Design Library is set to Auto-Hide, turn Auto-Hide off by clicking the push pin in the upper-right hand corner of the Design Library.

Adding Features to Design Library

Now that the appropriate folder has be located and the Design Library pane is open, you can add the desired features to the Design Library. In the FeatureManager, select the features while holding down the CTRL key.

While still holding the CTRL key, drag the features into the lower pane of the Design Library and drop them into the folder.

Add to Library PropertyManager

In the Items to Add section of the Add to Library PropertyManager, you will see a list of selected features that you are adding to the Design Library. This is your chance to make sure that you have added the correct features. you can add or remove additional features, if it is necessary.

In the Save To section of the Add to Library PropertyManager, enter the File Name that will be displayed in the Design Library. Also, ensure that the correct folder is selected in the Design Library folder window.

Lastly, add the Description that will be shown in the tooltip when you hover the mouse over the Design Library item.

Click the green check mark and the features will be added to the Design Library.

We’re Not Done Yet…

Next, I will cover how to add features from the Design Library onto a new part.

If you enjoyed this post, make sure you subscribe to my RSS feed!

Related posts brought to you by Yet Another Related Posts Plugin.