In this part of the guide, we’ll find out Altium create footprint process. The process of creating footprints in Altium is not complicated. We have the manual creation of libraries by placing pins, overlays, etc. on the sheet, additionally, the creator of Altium added two wizards to the program, which significantly accelerate the Altium create footprint process.
You can check our Tutorial Viedeo on youtube:
To start the process of creating a footprint, it is necessary to add a PCB library file to the project, it is done by clicking RMB on our project and selecting the Add New to Project> PCB Library option.
After selecting this option, a file with the extension .PCBlib will appear in the files of our project. To manage the PCB library files, select the PCB Library option from the bottom bar.
A window will appear, to which we manage PCB library files. A list of currently created libraries in a given library file is available here. We can add a new library, delete it, edit it and directly insert it into the PCB project.
Altium Create Footprint through the Footprint Wizard function
The Footprint Wizard libraries can be found in the Tools> Footprint Wizard.
After enabling the wizard, we have access to creating PCB libraries of various elements. This wizard is great for creating a footprint for capacitors, resistors, diodes, BGA circuits and other available components on the wizard list.
Creating a THT capacitor PCB library
In this example, we will create a PCB library of the THT capacitor. To create such an element, the basis is to have a catalog note with housing and lead dimensions.
On the list in the Footprint Wizard, in our case, we select the capacitor and the unit of measure mm, because in our catalog item sheet the units are in mm. In the next window select the assembly method, in this case, it is Through Hole because the element is made in the THT method.
You can also choose Surface Mount for elements in SMD assembly.
The next step is to set the dimensions of the capacitor pad. Using the catalog notice, we define the dimensions.
To determine the dimensions of the hole we use the formula for the minimum dimension:
Minimum Hole Size = Maximum Lead Diameter + 0.25mm (for Level A of IPC-2222)
Minimum Hole Size = Maximum Lead Diameter + 0.20mm (for Level B of IPC-2222)
Minimum Hole Size = Maximum Lead Diameter + 0.15mm (for Level C of IPC-2222)
In our case, I used the first formula, that is:
Minimum Hole Size = 0.5mm + 0.25mm = 0.75mm
However, to determine the dimensions of the pad we use the formula:
Pad Diameter = Minimum Hole Size + 0.1mm + 0.60mm (for Level A of IPC-2221)
Pad Diameter = Minimum Hole Size + 0.1mm + 0.50mm (for Level B of IPC-2221)
Pad Diameter = Minimum Hole Size + 0.1mm + 0.40mm (for Level C of IPC-2221)
Here I also used the first formula:
Pad Diameter = 0.75mm + 0.1mm + 0.6mm = 1.45mm
In this way, the condenser holes and pads were fixed.
The next step is to determine the distance of the pad.
In this case, it is 2mm, for a capacitor with a capacity of 220uF.
The next step is to set the type of construction of capacitor leads, overlay and type of PCB assembly.
In this case, set to the Polarised mode when we have a specific direction of conduction, the type of assembly on the radial and the overlay of the element is the circle. Thanks to these settings, you can also create elements such as external quartz because they have the same lead outlines and contours available.
Now it’s time to create outline contours. We specify it using the diameter dimension, in the Altium program the radius of the circle is given.
After completing these steps, all you have to do is give the name to the item and finish the work of the Footprint Wizard.
As a result of these operations, a THT polarized condenser footprint was created with dimensions determined on the basis of the datasheet.
There was only a slight modification consisting in moving the + sign from the left side indicating the polarization direction of the element.
The capacitor PCB library has been made. The last step is to import the footprint into the schema library.
We import footprint in the schema library file (if you do not know how to create it see Altium schematic library tutorial) by clicking the Add Footprint button.