Industry standards have been a boon for the electronics industry. These standards give designers assurance that the components they select can be reused across their designs, specifications will be consistent, and that IPC-compliant manufacturers can build their boards using standard processes. It’s all about increasing productivity and ensuring your devices will work as you intended.
The IPC 7350 series of standards (specifically, IPC 7351B) specifies generic physical design parameters of land patterns for surface mount components. Different types of components require specific footprints if they are to comply with this standard. Manufacturers work within these standards to ensure that products meet quality and reliability requirements, as well as reducing the amount of rework or scrap.
When designing your PCB to be compliant with IPC 7351B standards, you may find that your surface mount components are not compliant with the standardized land geometry. You can certainly use the component, but you might incur extra design costs from your manufacturer as they need to adapt their process to work with your particular component. If you’re working with a customized, proprietary component, it is a good idea to design the component so that it is IPC compliant.
Creating a Component With an IPC Compliant Footprint
Not all components are designed with IPC compliant footprints. Thankfully, the best PCB design software packages have the CAD tools that allow you to work with these components, so long as you apply some simple design strategies. For example, the pitch between landing pads may not be compatible with standard trace widths, and you’ll need to modify this setting in your design software if you intend to use these non-compliant components.
If you’re looking to avoid any placement or routing problems that can arise when working with custom components, you can skip the hassle and immediately create an IPC compliant footprint for your component. The IPC Compliant Footprint Wizard is available in Altium Designer as an application extension. This wizard uses templates to generate compliant footprints for your components and saves a huge amount of time compared to creating a component manually.
To access the wizard, you’ll need to create a new PCB library file. You can create this as a standalone file or as an addition to an existing project. With this new window active, you’ll need to click on the “Tools” menu and select “IPC Compliant Footprint Wizard”. You’ll see options to create many different component footprints. For this example, we’ll use the CQFP package.
Selecting a component from the IPC Compliant Footprint Wizard in Altium Designer
After you click “Next”, you’ll be able to define your package dimensions. You can select the package dimensions you need for your custom component. You’ll also get 2D and 3D previews of your component footprint and you can generate a preview of your STEP model for this component.
Defining the dimensions for a component footprint in Altium Designer
The following screen will let you define minimum and maximum values for the lead width range and the number of pins required for this component. The wizard will calculate the required lead span range and the lead length range for the lead widths and number of pins you specified. You can also enter your own values on this screen. Once you click “Next”, the wizard will show you the maximum and minimum gull-wing values for this component.
The next two screens allow you to define tolerances for this component. You’ll have some freedom to adjust these values based on the specifications from your component manufacturer. You’ll also see a screen that shows the pad dimensions for this component, and you’ll have the ability to define the silkscreen width, courtyard and assembly information, and component body information. Many of these values will be calculated for you based on the IPC specifications, and you should use these values if you want your component footprint to be compliant.
The final screen allows you to save your new component information in a PCB library. You can embed it in the current new library that is open in the background, or you can create a new library file for this component. You can also export a 3D STEP or Parasolid model for your component. Click “Next” and then “Finish” to complete the wizard.
Saving your component information and models in Altium Designer
Once with wizard finishes processing, you’ll get access to 2D and 3D views of your finished component. Go to the “View” menu and select “3D Layout Mode” or press “3” on your keyboard to see your new component in 3D.
3D view of your new custom component
This new component has been saved in a .PcbLib file, and it’s been given the name “CustomCQFP.PcbLib”.
Creating a Symbol for Your New IPC Compliant Component
Once you’ve created the footprint for your new component, you’ll need to create a symbol for it so that you can use the component in a schematic. First, you’ll need to create a new integrated library project. Click on File -> New -> Project -> Integrated Library to load this new project. You’ll then need to add the .PcbLib file you created in the previous section to this project. You can drag this file into the integrated library project if you still have it open in the navigator, or you can open this file manually.
Now you’ll need to add a new schematic library to your new integrated library project by clicking File -> New -> Library -> Schematic Library. You’ll need the .PcbLib file and the .SchLib files in this project in order to create a link between the schematic symbol and the component footprint that will appear in your layout. To link the two files, click on Tools -> Model Manager. This will bring up the window shown below.
The Model Manager dialog in Altium Designer
The footprint is linked to the schematic by click “Add Footprint”. Another window will appear that allows you to select a .PcbLib file from your local machine or from the current integrated library project. Since the CustomCQFP.PcbLib file was already added to the project, you can click the “Browse” button and select the CustomCQFP component directly without searching for it on your hard drive.
Linking your PCB model to your schematic library
If you have the schematic symbol generation tool installed, you can access the extension from the “Symbol Wizard” option in the “Tools” menu. You’ll see the symbol creation wizard appear. This dialog lets you define the pin layout that you’ll see in the schematic symbol. You can also choose the pin arrangement that appears in the schematic symbol. You can choose whichever arrangement will make it easiest to make connections with your other components.
If you have a small number of pins in your component, you can configure each manually if you like. However, for components with a large number of pins, you can actually write out the pin information in Excel and copy it into the pin table in the Symbol Wizard rather than scrolling through a large table and defining each pin manually. This makes it very easy to define groups of pins quickly. You can also easily define the electrical properties (Input, Power, Output, I/O, etc.), reference designators, and display names.
Once you have built the symbol for your new part and defined the functionality of each pin, you can place it in the schematic library by clicking the “Place” button, followed by “Place Symbol”. This will place the symbol in your schematic library, and it will now be linked to your new compliant footprint.
The schematic symbol for the CustomCQFP component
If you need to make changes to your schematic symbol, just click on the “SCH Library” tab in the “Projects” panel on the left side of the screen. From here, you can link supplier information and edit your pin information. You can also customize the size of the pins that appear in the schematic symbol. Once you’re ready to compile your integrated library, click on the “Project” menu, followed by “Compile Integrated Library”. This will save your new library in your project folder.
Once you’ve finished building your components and compiling your integrated library, you can add install your new library and start adding your IPC compliant components to your PCB. Note that these tools only create structural models and schematic symbols for your components. You’ll still need to add electrical simulation models to your components if you want to use them with the signal integrity and PDNA tools in Altium Designer.
Altium Designer unifies information in your component libraries and your design rules, allowing you to work with components that have any footprint. The integrated environment in Altium Designer allows all you to build models for your custom components that meet the basic IPC standards, and the ultra-accurate 2D and 3D CAD tools make it easy to incorporate these components into your PCB.
If you want to learn more about Altium Designer, talk to an Altium expert today.
About the AuthorVisit Website More Content by Altium Designer