Companies build their Inventor custom content libraries for various reasons. Some will create them to hold their internal custom parts, others will copy existing libraries and change their default part numbers and filenames to suit their company standards. I would like to give you another reason and that is the ability to add parametric features to your custom libraries. I am going to show you the simple method of adding parametric features to every member of your custom library family with one easy command.
I am going to create a custom content library of ANSI equal leg angles that contain two parametric features. One is actually two slots at each end of the angle that are centered on one leg but can parametrically and can be adjusted in size and location for each piece of angle steel placed in an assembly. The second feature is the parametric embossing of a part number on the opposite leg of the angle. Here is a screen shot of my part.
Before I continue, I am assuming everyone knows how I created my custom content library by coping the Inventor ANSI equal leg angle standard library to make it editable. Drop me a line if you need a separate article on that process.
Next I created an assembly using inch units. I place a piece of angle, in my assembly, from my new custom library. I used a piece of 2 x 2 x 1/4 but it is not really important what size you choose. I hate to work on small parts if I do not have to. The angle has to be saved as a custom library part so I gave it a name of Angle Template Part just to make it easy to find. If you would like to use this process on a custom library that does not, by default, save the placed component as a custom part, just select "As Custom" during the placement process.
Open up the part and add your desired parametric features. Be sure to use the User Parameters already in the model to help you achieve what you want. I used the G_H (Leg Depth) variable to keep my slot centered for all angles in the family. Features and parameters are up to you. You could place bolting holes, cutouts, patterns or addition features anything you desire.
For the parametric label, I used a Text user parameter with values in a Multi-List, assigned it to sketched text, constrained to a certain place on the angle leg, and then embossed it. When a piece of steel is place in an assembly from my custom library, a quick parameter change and I have a new label. Save the part, you will use it in the next step.
All of this preparation has lead me up to what this article is all about. I want to add all of these features and any other modifications such as color, custom properties, etc. to all the members of my custom content library in one quick step. I saved the part I have been adding to and closed it. I go into the Content Center Editor and locate my custom library, right click on the family I am editing and chose "Replace Family Template" from the context menu.
The program may give you a warning about replacing the template on a linked library, click Yes and continue. It will then ask you to select the part you saved out of the custom library and have been modifying, in my case it was Angle Template Part. After selecting Open, you will see a message "Publish was Successful" and you are done.
The next time you place a part from this custom content family in your assembly, it will have all the features you included in your template part. Best of all the features are applied to every member (size) in the custom library with only one simple command. Save your template part so you can add or modify features as needed and follow the same process to update your library members.
This process adds a whole new dimension to Inventor Custom Content Libraries. See what you can dream up in your design process to take advantage of this process.