Create your own template symbol?

[onesixright]

When you go to "C:\Users\Public\Documents\Altium\CS\Templates\SchLib" you see the a bunch of library files (like Battery, Diode, etc.).

They have all the same names of the symbols that you can select via "Home > Symbol" (this only shows when you have a 'schematic library document' active/open)

So, is there anyway to create your own symbol (templates)?

I tried copying one file and changing it, but (even after restart CS) it doesn't show up. I also tried creating a new Schematic Library, but that also didn't work. 

Maybe its locked down in CS?

Much obliged!

[JamesH-AltiumOfficial]

Hi onesixright,

There are no templates for component symbols or footprints in CircuitStudio. It's not locked down as such because that's not a general feature in Altium products unless you're using the commercial Altium Vault which has a powerful component template feature with unit-aware parameters etc., and is used with Altium Designer.

The SchLib folder is there for helping beginners in getting started with a few generic symbols that could be used if they don't know how to draw symbols from scratch. But it is very basic so I've never mentioned its existence to anyone for this purpose.

Schematic Templates

The Schematics themselves can be setup with a template so that when a new schematic is created it is based on the template design.

Templates in C:\Users\Public\Documents\Altium\CS\Templates have the extension *.SchDot and can be copied and given a new name so that you can modify it to your own template.

Open the file (e.g. drag the file from C:\Users\Public\Documents\Altium\CS\Templates onto CircuitStudio) and ensure the file is shown in the Projects panel with the SchDot extension (not SchDoc).

Make the modifications to the template and save it into the Templates folder.

You can apply this template to existing schematics by using Projects > Template, Update Current Template, or you can choose the new template. Templates can also be set in the Document Options.

You can apply this template to any new schematics you'll create in the future by opening File > System Preferences, then go to Schematic > General and choose the template file from the Template drop down list.

Templates can be created as a new file:
Add a new Schematic and choose Save As. In the Save as type drop down, choose Advanced Schematic template (*.SchDot)
It's recommended to save it into the C:\Users\Public\Documents\Altium\CS\Templates folder, but you can also have project tempates if you wish.
Press O to open Document Options and click the Template tab.
Press Clear Template - this step may be necessary if you can't edit the template primitives.

Slightly off-topic but hopefully helpful; Here's some info about getting extra libraries in CircuitStudio:

Vault Explorer

Built into CircuitStudio is the Vault Explorer. This allows Altium Design Content components to be used directly in your designs. They're not editable components but they are stored in the SchDoc and CSPcbDoc files once they're placed on the schematic and updated to the PCB. So they exist in your designs for outputs or printing, even if you're offline.

You must be Signed in to use the Vault Explorer. View > Start shows the Home page. From there use the My Account drop down to sign in if you're not already.

Enable the content by using File > System Preferences, in the tree: expand Data Management > Vaults. If no vault is listed, click the Add Altium Content Vault button. Click OK to close Preferences.

File > Vault Explorer. Make the panel a bit deeper so that you can click the horizontal bar and expand the list to show more than one Item (component). Components have a blue icon. Drag one of them to your schematic and it will place it where you drag the mouse.

Use Tools > Annotate > Annotate Schematics Quietly to change *? to a proper part designator like J1. (The search field at the top right of the screen can find this command by typing quiet into it and hitting Enter.)

When you update your PCB document (Home > Project), the footprint will be automatically downloaded from the Altium Content Vault onto your PCB.

Design Content

Libraries can also be downloaded in order to edit them or to use them completely offline. Many of the components found in the Vault Explorer can be downloaded as follows. Altium's editable Design Content is available for anyone who registers, directly from the design content website, but actually does not require an AltiumLive account. Use the step-by-step guide below to download IntLib files and use or edit them in CircuitStudio.

It's not immediately obvious, so here are the instructions to do this:

1. Open https://designcontent.live.altium.com/#UnifiedComponents in your browser.

2. Register with First Name, Last Name, Email address and PCB Layout Tool

3. Receive the email containing a link and use the link in each web browser that you intend to download content.
   - a cookie will be saved in the browser so that you may download other libraries without registering each time
   - repeat for each type of browser you wish to use, e.g. Firefox or Chrome

4. The file downloads as a zip archive. This must be extracted to your drive prior to use in CircuitStudio.
   - e.g. click on the downloaded *.zip file and copy and paste the *.IntLib (Integrated Library) file to a folder on your PC.

5. Drag the *.IntLib onto CircuitStudio and Choose Extract Sources
   - the Projects panel will show a LibPkg project containing a SchLib and PcbLib file.

6. Special note for versions of CircuitStudio 1.3 and below: To allow CircuitStudio to locate the footprints during updating the board, these two files should be installed in the Libraries panel, or alternatively you may drag these two files into your project: SchLib and PcbLib.
   - CircuitStudio 1.4 (in Beta at time of posting; due for release in a few weeks) works better with libraries that are not in the project or are not installed in the libraries panel.

7. Edit the libraries. Often you only want one device when you've downloaded the family
   - you may choose to copy a Schematic component to your own custom library
   - don't forget to also copy the corresponding footprint(s) from the downloaded PcbLib to your custom footprint library.
   - edit the originals or copy and paste
   - components (symbols) can be copied from a schematic to a schematic library (change the Designator back to U? or similar)
   - components (footprints) can be copied from a PCB to a PCB library (if the footprint is locked, unlock it so you can select it and copy)

Octopart Common Parts Library

Octopart.com is a website owned by Altium and the library can be searched here: https://octopart.com/common-parts-library
The site was purchased in 2015 and is being used to enhance Altium's product range with richer component data and BOM and analysis tools. This section of Octopart.com is for: "The Common Parts Library for Production is a set of commonly used electronic components for designing and manufacturing connected device products."

To get these libraries, go to http://www.snapeda.com/libraries/octopart/common-parts-library/ and sign up (free).
Click Download Library and choose Altium as the format, to download Common-Parts-Library-Altium.lia

Follow these steps to import the P-CAD library into CircuitStudio:

Open a project or choose File > New Project > PCB Project, give it a name and click OK to create.
Select File > Import
Choose P-CAD Libraries (*.LIA; *LIB) in the drop down list and browse for the downloaded .Lia file.
Click Open to start the import.
When this runs the PCB library window will flicker quite intensely for several minutes, then the schematic library loads within a few more seconds, then a dialog displays with "Done".

Best regards,

James Harriman
Altium

[onesixright]

Hello James,

Thank you for you extensive reply!

Just to make sure we are on the same page, I added a screenshot.

I changed (added some text) to the Battery.SchLib, now when I click the Battery symbol on the toolbar, I do see the changed symbol. So apparently, the symbols in the toolbar are linked to these files. My thought would be that if you add you own symbols to this a folder, they would show up in the toolbar.

Thanks!

[JamesH-AltiumOfficial]

Hi onesixright,

Thank you, I'm really glad to have engaged in this conversation since I did not know these were used for the symbol button! There is always something new to learn...

In this case you can't add any more because the buttons aren't customizable but the existing symbol libraries can be edited as you've discovered.

Some comments:
 - If you edit them you should back them up to a folder outside of the Altium\CS folder, since the uninstall program will remove all files in there.
 - It places the symbol and sets the Default Designator and Default Comment and also imports any Parameters if they are visible in the Templates file.
 - It doesn't import the models, i.e. you can't specify footprints and make this like a full component template.

Best regards,

James Harriman
Altium

[onesixright]

Hi James,

Every day you learn something, is a good day! ;-)

Thank you for the feedback, its clear now. Maybe in 2.0? :-)

Kind regards,

--
R

[slowertech]

I like this idea. It would be nice if we could customize or expand the template symbols in a future update.