Introduction
So far in lab, whenever we’ve needed a symbol or footprint, we have been using components from the Altium workspace library. When you are designing you own PCBs, you are going to want to use parts that don’t already exist in your library, and you won’t have somebody else to create parts for you (unless you are working in a company that has a dedicated librarian). So, we need to figure out how to do these things for ourselves.
As a reminder, a symbol is the thing that we put on a schematic that indicates its electrical connectivity, while a footprint defines the physical features of how the board is made.
Creating a workspace component
Your components don’t have to live in a workspace, but workspaces integrate really well with Altium, so we’ll use that. Open the components panel (Panels->Components) and click Create component (or if you don’t see it Hamburger menu->Create Component). Normally, you would select the appropriate folder to do this in, but here make sure to select the RECITATION_10 folder.
Now, name it YourKerb_example1 and set the type to also be RECITATION_10.
A super simple example
Creating a symbol
We’re going to start off with a trivially simple part: a simple, 2 pin SMD capacitor. Hit the dropwon under Add Symbol and select New. Open properties (Panels->Properties). Give it the default reference designator C?. Also uncheck the eye next to the Name property.
First, let’s draw out the graphical part of the symbol. We will just draw a typical capacitor symbol using the line tool (on the right toolbar or Place->Draw Lines). You only need to draw the plates, we’ll add the pins next. It might take a while to figure out what is a reasonable sizing. Here, I am using lines of length 400 mils.
We’ve completed the graphics for our symbol, but we are still missing the most important part: the pins. The pins are the actual connection points for the wires. Go to Place->Pins. Place down two pins and configure them to have Pin Name and Pin Number to 1 and 2, and leave the Electrical Type to Passive. We’ll talk more about the electrical type in a more complex example, but it essentially just gives the ERC information to catch potential mistakes. There’s a x-shaped mark on one end of the pins. Make sure that this faces out since this is the point where the wire connects.
Now, make sure to save your symbol.
Footprint creation
Let’s move on to creating a footprint. We’ll stick with a simple SMD capacitor, specifically an 0603 part. Create a new footprint like you created a new symbol.
We will begin by placing a pad (from the right toolbar or Place-> Pad). Place this on the origin. Now, we must size it correctly. We will size it based on this recommended land pattern from a Murata datasheet.
Select the pad and open Properties. Set the Designator to 1 and the layer to Top Layer, then scroll down to the Pad Stack section. Change the Shape to rectangular and set the X size and Y size appropriately. With a little bit of math, we can figure out that the pad width is 1.0 mm. If you have your units set to mils instead of mm, you can just type mm in the box and it will automatically convert. Also make sure that the Paste is Enabled and the Tented option is not set for the Soldermask.
Duplicate it, change the new pad to number 2, and place it according to the footprint drawing. This requires us to place it 2mm to the right of the 1st pad, which we can achieve either by using the grid or directly entering coordinates in properties.
At this point, you might typically add some info on the mechanical layers to indicate things like courtyards or 3D body information. We will skip this, though it’s something to be aware of if you want to make really great footprints.
We can also add a couple of lines on the Top Overlay layer to help indicate how the resistor should be placed. You might want to choose a thinner line width than the default.
Great! We’re done with this footprint. You could also add 3D information to this, but that’s beyond the scope of what we can conver in recitation.
Importing External Models
The process we just went through is kinda annoying, and would be hugely time consuming if we had to do if for every part we use on a board. Luckily, a lot of time there are freely available models online. Let’s look at how to import models using the op-amp we used in lab AD8592 on DigiKey.
On DigiKey (and some other supplier websites), you can click the link listed under EDA/CAD Models to get these models. Click that link and download the UltraLibrarian models. Then extract the ZIP folder. You’ll notice that there is both a schematic library and pcb library. We could theoretically leave this as a separate library, but that becomes messy, so let’s merge these into our workspace library.
Go to File->Library Importer. Select Choose a File then navigate to what you just downloaded and select both the .SchLib and .PcbLib files. In Properties, change the Component Type to RECIATION_10. Also, make sure the Part Choices Mapping matches what is shown in the image.
Now, hit Validate which should only produce one warning (because we already have something with the same part number in the library). Errors should be addressed before proceeding.
Finally, hit Import. At this point, you should normally find your component in the library, and check that the symbol and footprint match the datasheet and also make any other edits you wish to make. However, we will skip this because you have all imported the same part and it would be difficult to tell whose is whose.
Example 2
Altium has a couple of wizards that make creating standard symbols and footprints very easy. So that we can play around with this feature, let’s use a fake part that we’ll call the ASoPD LT9999. This part has an SOT23-6 footprint, and the following pinout:
| Pin Name | Pin # | Description |
|---|---|---|
| VIN | 1 | Supply voltage |
| VOUT | 2 | Output voltage |
| PG | 3 | Power good (open drain) |
| SCL | 4 | I2C clock |
| SDA | 5 | I2C data |
| GND | 6 | Ground |
Just like we did for the first example, create an Example 2 component in the Recitation_10 folder.
Creating the symbol
First let’s create the symbol for this. Click Wizard... under Add Symbol. Enter the required info using the above pinout. It should look something like this:
Here’s a quick summary of what the Electrical Types are doing here (mostly for the ERC):
- Power: This tells Alitum that this pin will be connected to power nets.
- Open collector: Same as Open Drain. This is used when the pin can pull down a net, but it needs an external resistor to pull it up.
- I/O: Used when there is Bidirectional information flow (SCL can be bidirectional because of clock stretching)
The open collector type is a bit odd, and is probably mostly useful for telling the user that it is open drain/collector, rather than it being used for the ERC. It’s probably best to prioritize another pin type if it also fits that category (like the I2C pins).
After the wizard has generated your symbol, you can arrange the pins however you like. However, this is a fake device, so there’s not necessarily a sense of what’s logical for pin placement here. In Properties make sure to set the designator to U?
Footprint Wizard
The last thing we have to do for this is to create a footprint, but SOT23-6 is a standard footprint that we can generate using Altium! Click Wizard... under Add Footprint. For the Component Type, select SOT23. Enter the dimensions for the footprint according to this drawing.
Make sure to change the Package Type to SOT23 6-lead.
You should enter these general dimensions and the pin dimensions, but it’s fine to leave everything else as the default.
And easy as that, we are done.
Component Properties
Now, let’s add some properties. Normally, we’d just add a manufacturer link, and most of the relevant properties would automatically populate. However, since this is a fake part, we’ll link it to the LM358DT for demonstration purposes. Back on the component tab, select Add... under Part Choices.
Then, search for the LM358DT, select the first option, and press OK.
Finally, select OK under Use Component Data. Now, all of the part information automatically gets imported as parameters.
Extra Practice
If we have extra time in recitation, try creating some of these parts (which actually don’t have good ECAD models readily available).
- Multi-unit symbol practice: Try creating a multi-unit symbol for the AD8592 using this guide
- Tricky footprint: You’ll have to carefully read the mechanical drawing EVU-E2AF25B54
Some notes
- Never blindly trust that the ECAD model you found online is accurate
- Never blindly trust yourself. It’s easy to make tiny dimensioning mistakes, which could necessitate a respin of the board. Always double check!