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.
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.
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.
As an example, we will use an LDO operational amplifier in a SOT23 enclosure.
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.
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.
The next window is also determining the dimensions, this time the pin and pad.
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.
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.
After passing the next steps where the program automatically determines the parameters, we get a ready footprint.
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.
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.
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.
We start drawing the contour from the point 0,0 to make it easier to calculate other dimensions.
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.
The finished outline is as follows.
To create mounting holes, click Place Via and insert it in the point 0,0.
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.
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.
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.
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.
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.
Go to Edit> Paste Special … This operation opens a menu with special paste options. In the next window, click Paste Array.
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.
Pasted pads are ready to rename them, which can be found in the catalog sheet.
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/