Skip to end of metadata
Go to start of metadata

You are viewing an old version of this page. View the current version.

Compare with Current View Page History

« Previous Version 11 Current »

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!

 Click here to expand...
  1. 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

  2. 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!

  3. Select “Create component”

  4. Select the applicable category for your new component

  5. Hit OK!

  6. 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.

 Click here to expand...
  1. 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

  2. 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.

  3. Turn on “Show only matching with template” and disable all imports except of parameters

  4. Confirm the accuracy of parameters against the datasheet

    1. Disable any parameters that are incorrect

  5. 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

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.

 Click here to expand...
  1. We start with previous steps completed and no symbol applied

  2. Select the dropdown under “Add Symbol” and select “Existing…”

  3. 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”

  4. Clicking on symbol names will open a preview of the symbol. If a symbol looks good, hit “OK”!

  5. 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.

 Click here to expand...
  1. 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

  2. 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.

  3. Open the schematic library file. Sometimes they may provide an “Integrated” library. Either work fine.

  4. Confirm the symbol is usable. In this case, there are some fixes needed, but overall it looks good.

  5. Create a blank symbol from your component by using the dropdown and selecting “New”

  6. Open properties and update the Designator and Name per https://nerdocs.atlassian.net/wiki/spaces/NER/pages/118718470/Vault+Guidelines#Symbols.1

  7. Return to the downloaded symbol. Use Ctrl + A to select all and Ctrl + C to copy

  8. Paste into the new symbol file

  9. 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.

  10. Save (Ctrl + S) and close the symbol file.

  11. 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!

  12. Open the menu to the top right of the symbol preview and click “Select Target Folder…”

  13. 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

  14. 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.

 Click here to expand...
  1. 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!

  2. Under the “Add Symbol” dropdown, click “New”

  3. With nothing selected (click blank space), open the Properties panel

  4. Set your properties. Primarily Designator and Name

  5. Right click the line icon to open the shapes menu and select the rectangle tool

  6. 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

  7. Select the pin tool from the toolbar

  8. 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

  9. Click the pause button to resume placement of the pin

  10. 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)

  11. Repeat #8-10 to populate all pins

    1. The tool will automatically increment the pin number for more rapid placement!

  12. Once all placed you may need to adjust your pin placement and block size. This is done via standard clicking and dragging

  13. Save (Ctrl + S) and close the symbol file.

  14. 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!

  15. Open the menu to the top right of the symbol preview and click “Select Target Folder…”

  16. 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

  17. 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 component 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.

 Click here to expand...
  1. Select the dropdown under “Add Footprint” and select “Existing…”

  2. An explorer window will open from which you can search for a footprint

    1. All footprints 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, “Resistors”

    3. For the ICs, such as AP2120N-3.3TRG1, footprints are sorted into package categories. For this linear regulator, it is a SOT-23, so we look in the SOT folder to find an existing footprint

  3. Clicking on symbol names will open a preview of the footprint. If a footprint looks good, hit “OK”!

  4. If the pins line up with the symbol, you’re done! If not, continue to step 5

    1. In the case of the linear regulator, the pin numbers do not line up so we need to go to step 5!

  5. If your symbol and footprint numbers don’t align, click the “Pin Swapping” button

  6. Update the footprint column to determine which footprint pin should be attached to each symbol pin

  7. If successful, the footprint will now show it has a custom mapping!

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 https://nerdocs.atlassian.net/wiki/spaces/NER/pages/118718470/Vault+Guidelines#Footprints.1 and to verify dimensions against the datasheet!

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

 Click here to expand...
  1. 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

  2. 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.

  3. Open the footprint library file. Sometimes they may provide an “Integrated” library. Either work fine.

  4. Confirm the footprint is usable. You may need to navigate to “PCB Library” and then select the footprint name to open the footprint.

  5. Create a blank footprint from your component by using the dropdown and selecting “New”

  6. Open the properties panel, open the “Footprint” tab, and update the Designator and Name per https://nerdocs.atlassian.net/wiki/spaces/NER/pages/118718470/Vault+Guidelines#Vault-Organization

  7. Confirm in the View Setup panel that the standard layers have been setup per https://nerdocs.atlassian.net/wiki/spaces/NER/pages/118718470/Vault+Guidelines#Layer-Pair-Setup. If your templates are set properly this will happen automatically.

  8. Return to the downloaded footprint. Use Ctrl + A to select all and then Ctrl + C to start a copy, then left click on the origin to set your copy reference point.

  9. Paste into the new footprint file using Ctrl + V to start pasting and click on the origin to confirm placement.

  10. Walk through each layer to confirm contents are in the correct layer and to make any necessary line width and placement adjustments

    1. Use single layer mode to simplify viewing layer by layer (Shift + S)

    2. Additionally, if any contents need to switch layers, select those elements and then use the properties panel to change their layer without having to copy/paste

  11. If your footprint does not include a 3D model, but the download does, add this now to the “Top Assembly” layer

    1. Start by opening the import window

    2. Navigate to your 3D model. In this case there was a separate folder in the download called “3D”

    3. Left click to place the model and then right click or escape to cancel placing more

    4. Manipulate the location as needed to get into place. Confirm it is in alignment in both 2D and 3D mode

  12. Make any final additions to reach full compliance to https://nerdocs.atlassian.net/wiki/spaces/NER/pages/118718470/Vault+Guidelines#Footprints.1. This may include adding pin 1 designator, adjusting pad shape, etc.

  13. Save (Ctrl + S) and close the footprint file.

  14. You should now see on the component your new component, including updated name!

    1. The name and 3D preview are good spot checks to make sure you didn’t forget major aspects

  15. Open the menu to the top right of the footprint preview and click “Select Target Folder…”

  16. Select where to store this footprint (within a subfolder of the Footprints folder) and click “OK”. For all common semiconductor devices, this is within the “ICs, Semiconductors” folder. In this case, “SOIC” is most fitting.

  17. Done! Your footprint 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 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.

 Click here to expand...
  1. Prepare yourself by finding the component drawing within the datasheet.

    1. This is usually within the last few pages

    2. Ideally, it has a recommended PCB layout!

  2. Create a blank footprint from your component by using the dropdown and selecting “New”

  3. Open the properties panel, open the “Footprint” tab, and update the Designator and Name per https://nerdocs.atlassian.net/wiki/spaces/NER/pages/118718470/Vault+Guidelines#Vault-Organization

  4. Confirm in the View Setup panel that the standard layers have been setup per https://nerdocs.atlassian.net/wiki/spaces/NER/pages/118718470/Vault+Guidelines#Layer-Pair-Setup. If your templates are set properly this will happen automatically.

  5. Start with pad placement

    1. Open the pad tool

    2. Hit Tab to pause placement and open properties

    3. Update your designator (pin number), pad size, and hole size as needed

    4. Place pads where needed. Adjust your grid size or utilize properties to enter coordinates

    5. Repeat as needed for each pad shape/size

      1. I highly recommend matching your footprint origin to the origin in the datasheet for easier dimension entering and comparison!

  6. Add anything else required by the datasheet. In this case, stitching vias and a pad shape modification

  7. Add your 3D model

    1. Open the 3D model tool

    2. Select your file and click “OK”

    3. Adjust as needed to align the model to the pads. Confirm it is in alignment in both 2D and 3D mode

  8. Define a component outline

    1. Open the line or rectangle tool

    2. Draw a shape matching the component body using the datasheet

      1. Sometimes, it is possible to just trace the boundary of the 3D model to form the component outline. This was not the case here.

  9. Add a courtyard

    1. Use the line or rectangle tool

    2. Add a courtyard defining the clearance required to the component, per https://nerdocs.atlassian.net/wiki/spaces/NER/pages/118718470/Vault+Guidelines#Courtyard

  10. Add a component center

    1. Set the origin to the center using “Edit” > “Set Reference” > “Center”

    2. Select the line tool

    3. Draw a symmetric plus marking the center, per https://nerdocs.atlassian.net/wiki/spaces/NER/pages/118718470/Vault+Guidelines#Component-Center

  11. Add silkscreen to the “Overlay” layer. This should include any markings useful for assembly, such as a pin 1 designator, alignment markings, etc

  12. Make any final additions to reach full compliance to https://nerdocs.atlassian.net/wiki/spaces/NER/pages/118718470/Vault+Guidelines#Footprints.1.

  13. Save (Ctrl + S) and close the footprint file.

  14. You should now see on the component your new component, including updated name!

    1. The name and 3D preview are good spot checks to make sure you didn’t forget major aspects

  15. Open the menu to the top right of the footprint preview and click “Select Target Folder…”

  16. Select where to store this footprint (within a subfolder of the Footprints folder) and click “OK”. For all common semiconductor devices, this is within the “ICs, Semiconductors” folder.

  17. Done! Your footprint will now show its full name and destination for saving

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:

  1. Under “Part Choices” click “Add…”

  2. By default, results will appear for the current part MPN, however click on the search bar to enter any other MPN or SPN

  3. 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!

  1. Open the Component panel and search for your part number

  2. Right click and access “Operations” > “Change State…”

  3. Ensure your “Next State” is set to “Promote 2 To Pending Review”. By default, this should be the case.

  4. Click Process!

  5. Click yes (no need for a comment on this one)

  6. 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.

  1. Click the “Pin Swapping” button

  2. Update the footprint column to determine which footprint pin should be attached to each symbol pin

  3. If successful, the footprint will now show it has a custom mapping!

If you have multiple footprints (for example a MOSFET that has a straight and 90 degree option), there will be multiple columns, each correlating to a footprint that can be independently configured

If you have multiple footprint pads intended for a single schematic pin, you can use commas to specify multiple!

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

RETURN TO HOME PAGE: Altium Designer

  • No labels