Making Parts for PCB Libraries

	This is a guide Welcome! This article is intended to guide you through an SSI process. While its authors have made efforts to make it useful, if you have questions, please ask the authors on Slack. They will be able to both help you and improve this resource for future SSI-ers. This article was written by Sasha Maldonado (@{{{display-name}}} ).

This article describes how to create a new part in SSI's Altium PCB component libraries. SSI maintains a collection of Altium component libraries, many of them derived from libraries generously donated to SSI by the Stanford Solar Car Project. This is designed to serve as both a reference, and a practical guide for how to turn a component with a datasheet into a schematic symbol with a corresponding PCB footprint.

This tutorial uses a template to show the keyboard shortcuts associated with certain tasks  first key → second key → third key → etc.. These shortcuts usually require you to have a file open in Altium and for your last click to have been in the edit window for that file (the large, central part of the screen). If you're having trouble getting a keyboard shortcut to work, click on an empty part of an open file and try again.

Introduction

The "Projects" pane, after opening SSI.libpkg.

Prior to creating a part, you should have installed and configured Altium and TortoiseSVN. In Altium, open the SSI Library project - SSI.libpkg, in SSI_SVN/libraries/intlib - with File → Open Project  f → j. Your "Projects" pane should now have a large number of .PcbLib and .SchLib files open (see right; open the projects pane with View → Workspace Panels → System → Projects  v → w → s → p if the "Projects" pane is not visible).

Altium has several different noteworthy types of libraries.

• Schematic libraries (.SchLib files) store schematic symbols and the components they correspond with. Schematic libraries contain schematic editor symbols, links to footprints (from PCB libraries; see below), mapping between the pins in the schematic symbol and pads on the footprint, and links to the part supplier (most often, Digi-Key)
• PCB libraries (.PcbLib files) contain the actual PCB layouts for library components. PCB libraries include footprints (the actual copper shapes and labels that will appear on the PCB) and 3D models of the associated packages.
• Integrated libraries (.LibPkg files) are Altium projects that combine schematic and PCB libraries.
• Compiled libraries (.IntLib files) are installable files that allow you to use library parts in schematics and PCBs. Every time a part is added to a library, the Integrated library will need to be recompiled before the part can be added to a PCB project.

For this tutorial, we will be mostly working with .SchLib and .PcbLib files. You will also need to open and compile the SSI.LibPkg file.

Locking in SVN

Right clicking on Connector.SchLib and scrolling down to Version Control brings up the "Lock" option.

Prior to adding a part to a library, it's important to "lock" the library in SVN so that other people using the library don't create a conflicted copy. Locking does keep other people from making library edits at the same time, so do not lock a library unless you will be immediately editing it, and, even if a symbol or component is not completely done, commit any libraries you've locked before stepping away for an extended period of time (see Recompiling and SVN Management). To lock any library, right click on it in the Projects pane, click "Version Control," and then "Lock"  right click → e → l. If you need to edit a locked library, mouse over the lock symbol in the Projects pane to see who has the lock, then message them in the #altium  Slack channel to ask if they still need the lock. You can override the lock, but doing so creates the risk of a conflict and will result in lost work if the lock is protecting ongoing changes.

What is a Part?

• 

  An example of a schematic symbol for an integrated circuit

• 

  The above schematic symbol corresponds to this real part, which would have a footprint with three holes - one for each pin.

• 

  The above schematic symbol could be copied to refer to this part as well, because it has the same number of pins and each pin serves the same function.

A part represents a real electronic component - a resistor, a connector, an integrated circuit, etc. A part is defined in Altium with a couple of things:

• A schematic symbol - a symbolic representation of the part which doesn't have to look like the actual, real-life part but should show how to electrically connect to it.
• A footprint - a drawing that shows what should appear on the manufactured printed circuit board. The footprint must match the dimensions for every feature of the part that will be soldered to the PCB, and usually also includes labels and a 3D model that help gauge how big the part is and how it's supposed to be installed.
• A supplier link - a reference to a vendor's page to sell the part, most often at digikey.com. These links mean that boards that use the part can automatically generate a cart of all of the parts on the board, making it easy to order the parts to assemble the board.

Every part has a unique schematic symbol in Altium, though similar parts often use the same drawings, with pins renumbered as needed. Every part in Altium also has a unique supplier link. Parts in Altium can use the same footprint, as they correspond to (usually) industry standard form-factors used for many different parts. There are thus many more schematic symbols than footprints.

Creating a New Schematic Symbol

Drawing a Symbol

To create a new schematic symbol, first find the relevant schematic library. Schematic libraries are sorted by function - i.e. power management integrated circuits (PMIC), diodes, etc. The table below serves as a reference.

Library Name	What Parts Go In It	Notes
capacitor.SchLib	Capacitors (all kinds).	Many ceramic capacitors are stored separately in sscp.dblib (ask in #altium  for details). Make sure to note the capacitor chemistry (i.e. CAP_CER for ceramic, CAP_TANT for tantalum (undesirable), CAP_ALUM for aluminum, etc.) in the schematic symbol name.
connector.SchLib	Connectors (all kinds).	Schematic symbol names should start with "CONN_".
diode.SchLib	Diodes (all kinds, including light emitting).	Note the type of diode in the symbol name ("LED_", "SCHOTTKY_", "ZENER_" - you don't need to include the word "diode").
fuse.SchLib	Fuses (both permanent and resetable).
ic_analog.SchLib	Integrated circuits for analog applications (op-amps, filters, etc.).	Note the general category of IC in the symbol name ("OP_AMP_", "FILTER_", etc.) NOT for analog-to-digital converters (see ic_data_converters below)
ic_data_converters.SchLib	Converting data from analog to digital or vice-versa (ADCs and DACs).	Begin the symbol name with "ADC_" or "DAC_" as appropriate.
ic_digital.SchLib	Digital integrated circuits i.e. logic gates. NOT for processors (see ic_processor below).	Begin the symbol name with the logical operation the IC performs ("AND_", "XOR_", etc.) where appropriate.
ic_interface.SchLib	ICs for connecting to standard communications interfaces i.e. CAN, Ethernet.
ic_pmic.SchLib	Power management integrated circuits, such as switching converters, linear regulators (LDOs), and battery protection.	Begin the symbol name with the converter type/topology ("LDO_", "BUCKBOOST_", "BUCK", etc.) where relevant.
ic_processor.SchLib	Processors (all kinds)
Inductor.SchLib	Inductors (all kinds) and transformers.	Begin the symbol name with "IND_".
mechanical.SchLib	Mechanical features, such as mounting screws, and test features, like test points.
miscellaneous.SchLib	Parts not properly described by any other category.	Use is discouraged, because it has a tendency to be a dumping ground - make sure there really isn't anything better.
modules.SchLib	Standalone modules i.e. prebuilt Arduino boards
Oscillator.SchLib	Oscillators and crystals.
Resistor.SchLib	Resistors not available in resistor.dblib	All 1% resistor values in standard surface mount sizes are stored in resistor.dblib. Prefix the symbol name with "RES_".
rf.SchLib	Radio frequency parts and antennas.	RF connectors should stay in connector.SchLib
sensor.SchLib	Sensors (all kinds)	Prefix the symbol name with the kind of sensor ("ACCEL_", "GYRO_", etc.)
transistor_bjt.SchLib	Bipolar junction transistors.	We have mercifully few of these.
transistor_fet.SchLib	Field effect transistors (all kinds).	Please note polarity by prefixing with "NFET_" or "PFET_" as appropriate.

A view of the SCH Library pane after opening the Connectors SchLib.

A pin in a schematic symbol. Note the small white dots on the left side mark where wires will connect in schematics; this pin is on the left side of an IC.

The pin settings dialogue brought up during pin placement.

Next, lock the library you'll be working with, and double click the library to open it. If not already visible, open the "SCH Library" pane  v → w → c → b and look at the top field, where there should be a list of symbols. Click "Add" to create a new symbol, giving it a name consistent with the names used in the library (this is poorly standardized, but typically consists of, in all caps, <type_of_component>_<manufacturer_name>_<manufacturer_part_number>). Your new part should then become active, bringing up a blank editing window.

Next, you'll draw out the graphics for your symbol. Begin by setting the snap grid of the editor (the grid of points it will allow for drawing) to 10 point spacing, by opening the snap grid settings  v → g → s and entering 10 for the snap grid size. This is not strictly required, and smaller grids can be used to create finer detail in symbols (5 and 2.5 are recommended), but all connection points for the symbol (added later) must be placed on a 10 point grid and thus symbols should be drawn to accommodate that.

For logic gates, transistors, and other components that traditionally have distinct schematic symbols, it is helpful to draw those symbols - you can often copy the graphics from an existing, similar part by simply opening the existing part from the symbols list in the SCH Library pane, selecting all of the symbol in the editing window and copying, then reopening and pasting into your own symbol. You should then delete all of the pins and replace them as described below. If no suitable symbol exists, draw a symbol by placing lines  p → l, referring to existing symbols for guidelines on size and color. Altium's documentation of the line tool is available here.

Integrated circuits are typically represented in schematics simply with rectangles; you can place a rectangle  p → r by specifying two opposite corners. Rectangles are easy to resize; it is recommended that you start with a large rectangle and downsize after placing pins.

Pins

Pins are how your symbol will be connected to wires when used in schematics. Enter the pin placement tool  p → p, but before clicking to place your first pin, bring up the pin placement settings window  tab. If designing a footprint for an IC, enter the pin name for the first pin in "Display Name," and set the "Designator" to the first pin's pin number (typically 1). If placing a pin for a symbol where a name should not appear, uncheck the "Visible" box by Display Name, and set the Designator to the appropriate number. Finally, set "Length" to 20, and exit the "Pin Properties" dialogue. You can now place your pin - make sure you are using a 10 point snap grid, as failing to do so can lead to errors in boards that use your symbol. After clicking to place your pin, you should automatically be able to place another pin, with the designator automatically incremented - enter Pin Properties  tab to set the Display Name (and Designator, if needed), and then place your next pin. Repeat until all pins are placed.

Next, resize rectangles and lines and move pins around until you're satisfied with the look of the symbol. You're done drawing the symbol! Make sure to save the .SchLib you're working on - if you're not going to immediately proceed to Creating a New Footprint and/or Finishing a Component, commit the library you were working on - this will release the lock and allow others to work on the library.

While this is the generic approach for drawing a schematic symbol, Altium also contains tools for automatically drawing certain types of symbols.

Creating a New Footprint

Footprints are the geometries of the actual layers that will be made on a printed circuit board. They correspond to the "packages" components come in - ie. SOIC, SOT-23, and many more - and so are often reusable between different components. While schematic libraries were sorted by function, footprints are sorted by series (QFN, DFN, etc.) and part type. If the package type marked on your component's datasheet doesn't clearly fit a series and isn't a passive (resistor, capacitor, or inductor) and isn't a sensor (appropriate if the symbol was made in sensor.SchLib) or module (i.e. a full microcontroller, like a Teensy board), it probably belongs in the Miscellaneous library.

As before, lock the library your footprint will be added to, then open the library. If not already visible, open the "PCB Library" pane  v → w → p → b.

The component you created a symbol for above may already have a footprint in a PCB library; search for it before starting work in the next two sections, and if it exists, skip to "Finishing a Component".

IPC Compliant Footprint Generator

The IPC Compliant Footprint Generator

If your component is a standard package, there's a good chance you'll be able to generate your footprint using Altium's IPC Compliant Footprint Generator. Open up the tool  t → i, click "next," and search through the default styles listed. If your component is from a supported series, the tool will make your life a lot easier. Select the relevant series, and you will be prompted for a number of dimensions that should be specified on your component's datasheet. Unspecified dimensions - thinks like heel spacing, solder fillet, and courtyard and keepout areas - can typically be left as their default values. If you have doubts, finish the generator and then measure the pads it produces - check to make sure their dimensions match the ones you intended. If in doubt, ask for a second pair of eyes to compare your part and the datasheet. Remember, other users will assume your part is right, so make sure it's right!

Drawing a Footprint

If the IPC Generator isn't an option, you can place pads manually  p → p and use the pad editor  tab to set their layer, size, shape, hole size (if applicable) and position (once placed). "Pad" refers to any distinct feature on a PCB that corresponds to a pin in the schematic view. This includes both surface mount and through hole pads.

When placing a pad, first set the designator to indicate what pad you're placing. The designator does not have to be a number, and should match the designator of any schematic pin it will be connected to. Multiple pads with the same designator''can''be placed, and will all connect to the relevant schematic pin. This is useful for creating a polygonal pad shape out of several rectangular pads, as well as components where a single electrical net connects to multiple physical pads - for example, a Teensy board, which has multiple identical GND pins.

After setting the designator, set the layer of the pad. "Top Layer" pads are surface mount pads (and will have their copper exposed appropriately); "Multi-layer" pads will expose copper on both sides of the board, and can thus have holes put through them. If making a multilayer pad, check off "Plated" - failing to do so will trigger errors and cause your through holes to just be... well, holes. Finally, set size and shape accordingly, and hit okay to return to placing your pad. One option is to place your pad where it needs to go - the current coordinates of your mouse and snap grid size and units are displayed in the upper left, and you can freely change the units  q and snap grid size  v → g → g as your pads require. Alternatively, simply place the correct number of pads, and then double click on each to reopen the pad editor and set their coordinates individually.

Select this option at the top of the "Place 3D Body" dialogue in order to load a STEP file

Optional but very strongly encouraged: One of the strengths of the SSI PCB libraries - and a special feature of Altium - is the use of 3D models for 3D renders of PCBs. Search online for a STEP file for your component; while far from guaranteed, many components have models freely available. If possible, download one. To insert it into your footprint, use the Place 3D Body tool  p → b, then select "Generic 3D Body" at the top of the window that pops up. Then click "Load from file..." and after a short import time, you should see your 3D model appear. You can now place it on your footprint. Enter 3D view  3 to make sure it's aligned properly; you can return to 2D view  2 to use the Rotation and Standoff Height options to correct its positioning, as needed.

Finally, using the line tool  p → l, mark the "Overlay" (silkscreen) layer in some way to indicate how to properly orient your component. Tracing out the corners or general outline of the part aids in distinguishing it from other nearby parts, and placing a dot or circle (perhaps using the "Full Circle" tool  p → u) near pin 1 or another directional feature helps ensure the component is installed correctly.

Finishing a Component

Pairing Schematic Symbols and Footprints

After clicking "Browse," this dialogue will appear. Note the dropdown containing all installed .PcbLibs

After finishing a schematic symbol and footprint, switch to the schematic symbol in the schematic library editor. In the "Editor" pane at the bottom of the screen, click "Add Footprint," then "Browse." From there, find the relevant PCB footprint library in the dropdown, and then the relevant footprint within the library. Double click the footprint to return to the "Add Footprint" dialogue, where the selected footprint's details will now be shown.

Click "Pin Map," and confirm that the pins on the schematic symbol match up appropriately with the pads on the footprint (if pins were given designators that correspond with their pad numbers, this should have happened automatically). If they don't match, edit the fields until they do. Multiple schematic pins can map to the same footprint pad, but not the other way around - for two pads to connect to the same pin, they must be given the same number in the PCB library editor.

Next, click OK. Your schematic symbol is now paired with a footprint! The footprint should now show up in the list of footprints at the bottom of the Editor pane.

Adding Supplier Links

Showing how to add a supplier link to a part. This supplier link, for a real Digi-Key part (a Tchaikovsky CD) would be a very bad choice to add to an automotive capacitor symbol, as the symbol does not represent the product in question.

The final step is to add a link to a supplier part, to allow for automated BOM ordering. Open the "Supplier Search" pane  v → w → s → u, and type in either the manufacturer's part number or (better, though less universally applicable) the Digi-Key part number. A number of vendor options should appear if the part is purchasable. Most SSI electronic components are purchased in small quantities from Digi-Key; therefore, look through the list and try to find a "cut tape" (purchasable in single units) version of the part, ideally sold by Digi-Key. Then, right click (see right) and select "Add Supplier Link and Parameters to <SYMBOL_NAME>." When this completes, an entry should appear in the "Supplier" section of the SCH Library pane  v → w → c → b.

You're done creating this component! Save the schematic library, and proceed to the final steps below.

Recompiling and SVN Management

Recompiling the Integrated Library

Before you can use your new part, you'll need to recompile the SSI library. Recompile using  c → c. The compilation process may take some time, and may throw errors at its conclusion. While that clearly means you can stop if any of those errors are on the part(s) you've added, it's best practice to try and fix them before finishing. A common error is a duplicate pin error, where two pins in a schematic symbol have the same designator. This can be easily corrected by changing one pin's designator. Make sure (if necessary) to change the pin mapping after doing so, by clicking on the paired footprint in the Editor pane to bring back the necessary dialogue. If you compile without errors on any parts you added, congratulations! Your component is now officially part of the SSI library. You'll just need to commit it to the SVN for others to use.

Commit Files to SVN

Committing files to the SSI Altium SVN is important for synchronizing files across users. Proper locking is required to keep commits simple and easy. If you've changed a single file, right click the changed library in the Projects pane, click "Version Control," and then "Commit"  right click → e → c. If you've changed 2 or more files, right click on SSI.LibPkg, click "Version Control," and then "Commit Whole Project." You'll be brought to a menu showing all of the files you've changed, which you should quickly check to make sure has all of the files you need to commit.

You will be prompted for a commit message; describe the changes made in at least 20 characters. This minimum is imposed in an attempt to keep people from entering commits without useful messages. It's easy to get around this, but you'll be a better person for telling other people what you did. Your commit should then quickly complete, your version control state will update, your lock on the library will be released, and within 15 minutes your commit should be automatically posted to Slack. You are now, actually, finally, done - assuming your commit proceeds successfully. In the event of a failure, poke the #altium  Slack channel, and we'll work together to sort it out.

There are several hundred parts in the whole Altium library, between the contributions of SSI and Stanford Solar Car members. The process you've just completed has been gone through many times - and you benefit from everyone who spent effort to do it correctly before you. You owe that same favor to the people who will use the library after you.