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.

Altium Create Footprint

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.

Altium Create Footprint

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.

Altium 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.

Altium Create Footprint

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.

Altium footprint wizard

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.

Altium footrpint wizard

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.

Altium footprint wizard

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.

Altium footprint wizard

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.

Altium footprint wizard

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.

altium create footprint

There was only a slight modification consisting in moving the + sign from the left side indicating the polarization direction of the element.

altium capacitor footprint

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.

altium capacitor footprint

After clicking, a window appears with the choice of the PCB library file. By clicking the Browse button, go to the Browse Libraries window. In this window, we choose our file with PCB libraries and previously generated footprint, and then we approve the operation.

altium pcb model

After all these steps we have ready to place on the schematic element with a PCB library and a schematic library.

Creating a PCB library through the IPC Compliant Footprint Wizard

The second wizard available is the more extensive IPC Compliant Footprint Wizard. We can create complicated elements in multi-pin housing. We also run it after clicking the Tools> IPC Compliant Footprint Wizard tab.

altium IPC Compliant Footprint Wizard

As an example, we will use an LDO operational amplifier in a SOT23 enclosure.

Sot23 datasheet

Its dimensions were obtained from the datasheet from the link http://www.ti.com/lit/ds/symlink/lmv321-n-q1.pdf

As you can see on the list, we have a large selection when it comes to the type of housing that we can create. In our case it is SOT23.

altium IPC Compliant Footprint Wizard

In the next window, we enter the basic dimensions of the housing, such as the width of the mechanical contour, height etc. The dimensions have a minimum and maximum range.

altium IPC Compliant Footprint WizardThe next window is also determining the dimensions, this time the pin and pad.

altium IPC Compliant Footprint Wizard

If we do not have information about any precise dimension and there is the option Calculated to leave this option checked, the program will calculate the correct dimensions for us.

altium IPC Compliant Footprint Wizard

In the next step, you can specify the precise dimensions of the pad, in this case, they are given in the datasheet, if you do not have them, you can select the option Calculated.

altium IPC Compliant Footprint Wizard

After passing the next steps where the program automatically determines the parameters, we get a ready footprint.

altium IPC Compliant Footprint Wizard

The library is ready to be added to the schematic library in the same way as it was given for the capacitor element.

Create footprint manual

The third way to create a footprint is to create it manually. To start this process, click on the Add button in the PCB Library menu.

Altium create footprint manual

After clicking, we get a blank sheet ready to place the pad, outlines and other parts of the element.

As an example, we will use a 2×16 characters LCD display. We will create a footprint based on the size of the pad and outline.

Altium create footprint manual

The first element will be the creation of an outline. The easiest way is to set a point 0,0 on the edge of the contour, thanks to which it will be easy to calculate individual dimensions.
You create a contour on the Top Overlay layer using the Line tool.

Altium create footprint manual

We start drawing the contour from the point 0,0 to make it easier to calculate other dimensions.

Altium create footprint manual

Enter the length of 80 mm and thus we have the finished upper outline of the element. We create the rest of the contour by copying an existing line and entering x and y points.

Altium create footprint manual

The finished outline is as follows.
To create mounting holes, click Place Via and insert it in the point 0,0.

Altium create footprint manual

In the Via parameters, set the position on the sheet, the size of the hole and the size of the entire Via along with the size of the pad, which was calculated as in the case of the capacitor pad 2.8 + 0.1 + 0.6 = 3.5mm.

Altium create footprint manual

After adding all the Via element presents itself as on the bottom.
The next step is adding Pad to the sheet. This is done via the Place Pad option from the menu.

Altium create footprint manual

After adding all the Via element presents itself as above.
The next step is adding Pad to the sheet. This is done via the Place Pad option from the menu.

Altium create footprint manual

Place the pad at the point 0,0 so that it is easy to place it in the right place, it should be Pad with number one, as the first Pin in the LCD.

Altium create footprint manual

If the first Pad is in the right place and has the Designator with number 1, we can proceed to copy.

Special copying is a very useful tool if you want to quickly duplicate the same elements as Pad. We copy the element in its middle, we get it by clicking after copying the cursor in the center of the Pad.

Altium create footprint manual

Go to Edit> Paste Special … This operation opens a menu with special paste options. In the next window, click Paste Array.

Altium create footprint manual

As the LCD has 16 pins, we copy 16 elements added every 1 in the X-axis with a distance of 2.54mm from each other. After clicking ok, click the cursor on the center of the first Pad to paste the rest of the elements.

Altium create footprint manual

Pasted pads are ready to rename them, which can be found in the catalog sheet.

Altium create footprint manual

Pad names are given, this is not necessary but useful in the general order of the scheme.
It is still necessary to change the pad size to 1mm in this gold pin example.
The footprint is ready to be added to the schematic library.

PCB libraries created for download

Altium has prepared a database in which we can find a lot of files ready to be downloaded.
Please visit:  https://designcontent.live.altium.com/