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

1 Component Creation Flow
2 1. Create from Template
3 2. Enter MPN and Import Data
4 3. Fill in Parameters
5 4. Symbol
6 5. Footprint
7 6. Add SPNs
8 7. Mark as Ready to Review
9 Appendix
- 9.1 Pin Swapping

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
1. 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
1. On popular distributors, such as Digikey, there is a dedicated field for MPN and a copy button
2. Ensure you do not use the supplier part number
Click the most accurate MPN/manufacturer to start the data import
1. 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
1. Disable any parameters that are incorrect
Click “OK”
1. 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

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!

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
1. All symbols are found in a dedicated folder within “Managed Content”
2. 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!

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.

For this demonstration, the NCV57001DWR2G isolated gate driver will be used.

Find a model. See 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 Vault Guidelines | Symbols.1
Return to the downloaded symbol. Use Ctrl + A to select all and Ctrl + C to copy
Paste into the new symbol file
This is a good time to make any fixes to make this compliant to 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!
1. 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 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.
1. 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: 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
1. 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)
1. 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
1. 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!
1. 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 (similar to symbol approach a).

b. Footprint Exists in Vault

It is always best to use an existing footprint. This allows for more rapid validation of components as our vault becomes more mature; if any component using shared footprint has a fabrication issue, this can be proactively resolved across all components using it!

For this approach I will demonstrate using the resistor and the AP2120N-3.3TRG1 linear regulator.

c. Importing a Footprint from Online

Often times a footprint is available for download either from the manufacturer directly or a 3rd party, which can save a lot of time for larger components. Just always remember to update the footprint to Vault Guidelines | Footprints.1 and to verify dimensions against the datasheet!

For this demonstration, the NCV57001DWR2G isolated gate driver will be used.

During Component Creation | 2. Enter MPN and Import Data you may be able to import a footprint along side the parameters. If you choose to do so, you must follow the above directions.

d. Creating a Footprint from Scratch

Sometimes a footprint just isn’t available anywhere. Or a component is made custom by us. Or quite simply, the footprint is simple enough that it’s faster from scratch.

For this demonstration, the ACS758KCB-150B-PFF-T high current sensor will be used.

6. Add SPNs

When an MPN is selected and is in the Altium database, an SPN will automatically be associated.

However, sometimes an MPN is not in the database, or there may be multiple variations on an MPN.

For example, for our resistors from Panasonics and connectors from Molex which have dashes in their part numbers (ERA-8AEB4993V) will sometimes yield different SPNs for when typed with or without.

More MPNs/SPNs can be added via:

Under “Part Choices” click “Add…”
By default, results will appear for the current part MPN, however click on the search bar to enter any other MPN or SPN
Select the matching option, and click “OK”

7. Mark as Ready to Review

Once finished, the component must be marked as ready for a Head EE to review!

Open the Component panel and search for your part number
Right click and access “Operations” > “Change State…”
Ensure your “Next State” is set to “Promote 2 To Pending Review”. By default, this should be the case.
Click Process!
Click yes (no need for a comment on this one)
Done! Your part should now have an orange state indicator

Appendix

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.

Click the “Pin Swapping” button
Update the footprint column to determine which footprint pin should be attached to each symbol pin
If successful, the footprint will now show it has a custom mapping!

Official Altium documentation: https://www.altium.com/documentation/altium-designer/single-component-editing#!edit_pin_mapping

RETURN TO HOME PAGE: Altium Designer