The core of Altium is its components. All manufacturer parts that may be used in a project are linked to design files that we must import or create to represent all aspects of a component, including schematic symbols, footprints, parameters and supplier numbers. This process can seem overly robust at times, but this enables improved time savings and reliability down the line in layout and in reuse of components in future projects.
CONTENTS
RETURN TO HOME PAGE: Altium Designer
Component Creation Flow
Most importantly, any method that gets you to a Vault Guidelines compliant component, works!
1. Create from Template
Creating from a template allows for certain parameters and assets to be automatically added for you.
Templates are made by us, so if anything seems odd, let an admin know and we can make edits!
Open the “Components” panel. Location depends on your configuration, but often is in the right sidebar. If not open, you can open it via the “Panels” button in the bottom right
Search for the component MPN you are trying to add
This is a check to make sure we don’t already have it made!
Select “Create component”
Select the applicable category for your new component
Hit OK!
Your new component, using the corresponding template, will now open.
2. Enter MPN and Import Data
Simply entering the manufacturer part number and selecting the associated manufacturer can jumpstart your component creation by importing parameters!
The below expand features this process for a new resistor.
Set the “Name” field to the manufacturer part number
On popular distributors, such as Digikey, there is a dedicated field for MPN and a copy button
Ensure you do not use the supplier part number
Click the most accurate MPN/manufacturer to start the data import
Note: If you just hit enter and not select a dropdown, no import will occur.
Turn on “Show only matching with template” and disable all imports except of parameters
Confirm the accuracy of parameters against the datasheet
Disable any parameters that are incorrect
Click “OK”
You should now have some parameters filled in and a “Part Choice” should be filled in
It is also possible to import a symbol and footprint from this step. Do not do this to start. We require first checking options A and B for each, before importing a symbol or footprint from here. See those sections for more info and then come back to this if an import is needed.
3. Fill in Parameters
Fill in the remaining parameters, if possible, from the datasheet
Not all parameters are required. All are recommended, but only the exclamation marked ones are required
4. Symbol
As shown in the flowchart, there are a few different ways to assign a symbol. Each lettered section is a different method, with the first being the simplest, and the last being the most comprehensive.
a. Default Symbol
Templates with common symbols, such as capacitors, resistors, and inductors, have a symbol automatically associated upon creating the component!
If this symbol is accurate to your component, you’re already done!
Some parts rated for higher power may have multiple electrically equivalent pins (a capacitor with 4 pins for example). Do not change the symbol for this. We address this with the footprint process.
b. Symbol Exists in Vault
Some components are semi-communized. For example, transformers which are often 1:1 but may be 1:1:1, both of which we have symbols for already. Another example is simple ICs, such as a 3 pin linear regulator (Vin, Vout, GND).
In any of these situations, it is always best to do a quick check of the vault for any symbol that may suit your part. For this approach I will demonstrate using the AP2120N-3.3TRG1 linear regulator.
We start with previous steps completed and no symbol applied
Select the dropdown under “Add Symbol” and select “Existing…”
An explorer window will open from which you can search for a symbol
All symbols are found in a dedicated folder within “Managed Content”
It is recommend to search in the path that matches (roughly) the type of component you are making. In this case, “Integrated Circuits (ICs)” > “PMIC - Linear Regulators”
Clicking on symbol names will open a preview of the symbol. If a symbol looks good, hit “OK”!
Done!
In this example you can see that the pin numbers do not align to the datasheet. This mismatch will be addressed in the footprint stage with https://nerdocs.atlassian.net/wiki/spaces/NER/pages/146243680/Component+Creation#Pin-Swapping.
c. Importing a Symbol from Online
Often times a symbol is available for download either from the manufacturer directly or a 3rd party, which can save a lot of time for larger components.
Given how non-standardized symbols are, it oftentimes is faster to make it yourself, but use your own past experiences and judgment to decide when you should or shouldn’t import!
For this demonstration, the NCV57001DWR2G isolated gate driver will be used.
Find a model. See https://nerdocs.atlassian.net/wiki/spaces/NER/pages/158073007/Altium+Reference#EDA-(Footprint-Sources) for places to look. In this case I found a download on the manufacturer’s website
Download the model. This often requires making a free account with whatever website is hosting the files. Depending on the website, you may also need to specify your software, which for us is Altium Designer.
Open the schematic library file. Sometimes they may provide an “Integrated” library. Either work fine.
Confirm the symbol is usable. In this case, there are some fixes needed, but overall it looks good.
Create a blank symbol from your component by using the dropdown and selecting “New”
Open properties and update the Designator and Name per https://nerdocs.atlassian.net/wiki/spaces/NER/pages/118718470/Vault+Guidelines#Symbols.1
Return to the downloaded symbol. Use
Ctrl + Ato select all andCtrl + Cto copy
Paste into the new symbol file
This is a good time to make any fixes to make this compliant to https://nerdocs.atlassian.net/wiki/spaces/NER/pages/118718470/Vault+Guidelines#Symbols.1. In this case no changes are needed, but sometimes pin types, color, or names may need updating.
Save (
Ctrl + S) and close the symbol file.
You should now see on the component your new component, including updated name!
The name and designator letter are great spot checks to make sure you didn’t forget the properties!
Open the menu to the top right of the symbol preview and click “Select Target Folder…”
Select where to store this symbol (within a subfolder of the Symbols folder) and click “OK”. In this case, “PMIC - Gate Driver” is the most accurate folder
Done! Your symbol will now show its full name and destination for saving
During https://nerdocs.atlassian.net/wiki/spaces/NER/pages/146243680/Component+Creation#2.-Enter-MPN-and-Import-Data you may be able to import a symbol along side the parameters. If you choose to do so, you must follow the above directions.
d. Creating a Symbol from Scratch
Sometimes a symbol just isn’t available anywhere. Or a component is made custom by us. Or quite simply, the symbol is simple enough it just makes more sense to make the symbol from scratch.
For this demonstration, the NCV57001DWR2G isolated gate driver will be used.
Prepare yourself by finding the component pinout within the datasheet.
This is usually within the first few pages, sometimes (like this one) are even on the first page!
Under the “Add Symbol” dropdown, click “New”
With nothing selected (click blank space), open the Properties panel
Set your properties. Primarily Designator and Name
Right click the line icon to open the shapes menu and select the rectangle tool
Make an initial box for the symbol. Requirements for color pallet and pin spacing are here: https://nerdocs.atlassian.net/wiki/spaces/NER/pages/118718470/Vault+Guidelines#Symbol-Layout
Select the pin tool from the toolbar
Press tab while the tool is running to set the pin number (designator) and name. These are based on the datasheet
You may additionally want to adjust the pin length (in increments of 100mils), confirm the type is set to passive, and decide to hide or show pin names and numbers
Click the pause button to resume placement of the pin
Orient and place the pin using standard controls (X and Y to mirror, space to rotate, left click to place, etc)
Note that the crosshairs while placing are where wires connect, not where the pin should connect to the box (name text should be in the yellow box, not outside)
Repeat #8-10 to populate all pins
The tool will automatically increment the pin number for more rapid placement!
Once all placed you may need to adjust your pin placement and block size. This is done via standard clicking and dragging
Save (
Ctrl + S) and close the symbol file.You should now see on the component your new component, including updated name!
The name and designator letter are great spot checks to make sure you didn’t forget the properties!
Open the menu to the top right of the symbol preview and click “Select Target Folder…”
Select where to store this symbol (within a subfolder of the Symbols folder) and click “OK”. In this case, “PMIC - Gate Driver” is the most accurate folder
Done! Your symbol will now show its full name and destination for saving
5. Footprint
As shown in the flowchart, there are a few different ways to assign a symbol. Each lettered section is a different method, with the first being the simplest, and the last being the most comprehensive.
a. Default Footprint
This currently isn’t a thing for any of our templates. But it could be! If so, just evaluate if the auto-populated footprint is accurate to your datasheet.
b. Footprint Exists in Vault
It is always best to use an existing footprint. This allows for
6. Add SPNs
{}
7. Mark as Ready to Review
{}
New version ^
Old version:
Creation via Clone
Cloning is used for components that have the same package and type (or otherwise just a notable enough amount of similarities) to existing components in the vault. For example resistors, where we may have hundreds 0603 resistors, but each has a different value, tolerance, and power rating (and more)!
This is arguably the easiest and fastest processes as it ideally only takes changing a few numeric values (no footprint work).
Read the dropdown for step-by-step:
Creation via Import/Download
Downloading and importing a component is the best way to bring in a new footprint, when the option is available. Not all components will have a footprint online to download, but when it exists it does save a lot of manual design. This process is for all components with footprints that we haven’t vaulted yet, but can be found online.
The most common sources of footprints online are:
SnapEDA
UltraLibrarian (Digikey)
SamacSys (Mouser)
Check https://nerdocs.atlassian.net/wiki/spaces/NER/pages/158073007/Altium+Reference#EDA-(Footprint-Sources) for the living page of sources!
This method allows for some time savings by avoiding the detailed drawing and dimension work, but still requires definition of the parameters and realignment of the footprint to NER standards.
Read the dropdown for step-by-step:
Creation from Datasheet/Scratch/Custom
Creation from scratch is the most annoying, but comprehensive method for creating a component footprint. This is typically used for components that don’t have data available online or components that NER has created custom.
As said above, this is the most tedious but thorough method of component creation.
Read the dropdown for step-by-step:
Pin Swapping
Pin swapping is a feature that Altium recently added allowing for symbols and footprints to be manually remapped on a per-component basis. This allows for more components to use fewer symbols and footprints!
The process is pretty simple, just click the pin swap button in the component edit view. Then use the table to remap.
{2 images, first showing the button, second showing the table}
Official Altium documentation: {need to find}
RETURN TO HOME PAGE: Altium Designer