Try now
Local PCB Library & Footprint Creation
With the help of the IPC Compliant Footprint Wizard, you can create any IPC components in just a few clicks by entering their parameters from the datasheet. Let’s create a footprint in the local library for component MBT3904DW1T1G whose symbol was created in Chapter 5.2. If you have closed the tab, open it from the Projects panel. As opposed to the approach with Altium 365, the local symbol and footprint are created in separate file libraries.
Select File > New > Library > PCB Library from the main menus to create a new local PCB library. The footprint editor will open in the design space. Open the Properties and PCB Library panels if they are not already open.
This component has a standard IPC SOT-636 package, so it can be created quickly with a few clicks using the IPC Compliant Footprint Wizard. Select Tools > IPC Compliant Footprint Wizard from the main menus to open the Wizard.
Tip: The IPC Compliant Footprint Wizard is also available while creating cloud components by clicking the Wizard button under the Footprint region.
Click Next in the IPC Compliant Footprint Wizard. Select SOT23 in the Component Types list then click Next.
Select SOT23 6-Lead from the Package Type drop-down menu. On this page of the Wizard, the dimensions of the component need to be defined, which can be found on the component datasheet. Set all values as shown in the figure below. Check the Generate STEP Model Preview option in the lower-left corner to automatically create a 3D model of the generated component. Click Next after you have entered all the values.
Enter all the values on the SOT23 Package Pin Dimensions page as shown in the figure below. This information is also available on the component datasheet. Click Next after you have entered all the values.
Click Next twice since there is no need to change the calculated values for Heel Spacing or the default value for Round Off Pitch.
On the Solder Fillets page, select Level B - Medium density from the Board density Level drop-down menu. Click Next.
Click Next three times since there is no need to change the calculated or default values on those pages.
On the Silkscreen Dimensions page, define the Silkscreen Line Width as 0.15 mm. Click Next.
On the Courtyard, Assembly and Component Body Information page, use the drop-downs to define the layers as shown in the figure below. Click Next.
On the Footprint Description page, enable the Use suggested values option and ensure that the Name and Description are as expected for the future footprint. Click Next.
On the Footprint Destination page, enable the Current PcbLib File option to save the generated footprint to the active PCB library. Enable the Produce 3D/STEP model and Embedded options. Click Finish to complete the footprint and exit the wizard.
After closing the Wizard, the generated footprint will appear in the list in the PCB Library panel. The generated footprint has all the necessary parameters, graphic designation, and assigned 3D models. Easy and very quick, wasn’t it?
Tip: You can add new footprints to your library by clicking the Add button below the Footprints list in the PCB Library panel.
Select File > Save from the main menus and save your library to a convenient location. Keep in mind that a local PCB library needs a schematic footprint library, so it would be a good practice to save those libraries in the same location. This is just one more reason why Altium 365 cloud component storage is more convenient and reliable. Close the PcbLib tab.
Now the two parts of our component - symbol and footprint - can be combined into a single component.
Open the SCH Library panel then select the MBT3904DW1T1G symbol that was created and saved in Chapter 5.2.
Click Add Footprint at the bottom of the editor to open the PCB Model dialog in which you can link the symbol with the created footprint.
In the PCB Model dialog, enable the Library path option in the PCB Library region and enter the location of the PCB Library file that you saved earlier.
Click Browse in the Footprint Model region to open the Browse Libraries dialog in which you can select the footprint.
Select the footprint you created then click OK.
The footprint displays at the bottom of the dialog. Click OK to close the dialog and apply this footprint to the symbol.
Tip: You can click the Pin Map button to open the Model Map dialog to check or edit the mapping of symbol-footprint pins.
Now the footprint is enabled for the selected symbol and our component is completely ready for the design. Select File > Save from the main menus to save the schematic library and close all tabs. Now there is nothing stopping you from taking your brilliant ideas and creating an actual device.
