CircuitStudio Libraries

Huh, I see half of my message is missing. Questions are.. Can I edit a component in the standard libraries, and can I add a new component to the standard libraries.

The answer is on principle yes, but ...

1) At first: the two original delivered libraries are only a collection of unsorted devices without visible order. I have rejected this two libraries after some hours of work.

2) this two libraries are from the "integrated library" type, file extension intlib. This is an extension of the old pcblib/schlib concept and integrates both libs into one integrated library-file. So no more looking: have I the according foorptint-library for my schlib available?

But the disadvantage: you can not directly edit the intlib-library, instead you first have to break the intlib into a separate schlib/pcblib, than edit what you want (add sch-parts or new footprints), than build both again together into the intlib-format. For me this makes constant ongoing work on parts in an integrated library not easy, personally I use mostly the old schlib/pcblib concept (I'm also not lucky with this, it's not easy to get some good ordering concept).

A description of the integrated library:

Component Management in CircuitStudio | Online Documentation for Altium Products

3) A good collection for libraries to start with: the original Altiumlibraries. They are also integrated libraries, but sorted with manufacturer and type. Much better starting point to modify some of this libraries.

https://techdocs.altium.com/display/ADOH/Download+Libraries

4) If you want to edit/modify such an integrated library:

File --> Open library --> select the intlib you want

You will get a question:

extract sources --> yes, if you want to edit/change something or look in the underlying pcb/schlib or copy some parts

install library  --> installs the intlib for use in your project, no modification

For the rebuilding process of the intlib: you have to search through the documentation on element14 or someone else may help.

Hi,

I agree that you would want to start with the non integrated library approach.  You will need to understand it anyway.  Later on, you can generate the integrated libraries from the separate ones if you choose to work that way.  I prefer to use non-integrated libraries and find it simpler.

To attempt to answer your actual question about adding parts to the standard libraries...you should create your own libraries and add in the parameters you care about.  Do not modify the provided standard/example libraries.  You can copy them and use them as starters.  Also, I attached a zip file with examples of libraries from my own development.

If you search the forum for library related information there are a few threads worth reading.

I think that every one has their own set of parameters they want to use in the libraries.  Some people like to include lots of parameters, others want minimal amount.

Here is a screen shot of what I use typically. In this case a low drop out regulator.  I have some extra parameters from a datasheet that make it convenient for me when picking parts out of libraries.  They are not required but I try not to get carried away and put the entire datasheet into the parameters.

For what it is worth, I attached a zip file with a schlib and pcblib with misc parts from libraries that I use.  I typically would have parts grouped into separate libraries for capacitors, resistors, ics, etc.

I should add to above that, I use the Component DNP parameter in schematic library to indicate if a part is not to be installed.  To do this I make the value (DNP) and then make it visible.  This shows up on the schematic and also I can use it to sort the BOM generation to group populated parts and non-populated parts.

Thank you Maik and Thomas. Sorry to take so long to reply. I had other matters to attend to.
I will try to digest what you say.

This is mostly an endorsement of the reply by mf_ibfeew and the link beginning and ending : https:.../Downloads+Libraries

That leads to a page that warns that its contents are obsolete, but that provides a link to the now current page(s).  After a few clicks, you'll have access to a huge, I mean HUGE!! resource of schematics and footprints of almost everything and anything your little heart could desire.  I mostly use old fashioned leaded devices, including plastic DIPs and resistors and capacitors big enough to see without a microscope, and these libraries have those, as well as the expected more modern surface mount devices.  Altium seem quite broad minded about providing access to this treasure, and I've downloaded several libraries, and they have worked brilliantly. 

Although the advice that it is possible to use them for getting started and to add your own components is correct, I urge caution.  It is almost certainly unnecessary, it is a BIG job, editing libraries is character building and not for people with a limited vocabulary of rude words, there is a big risk that a tiny mistake will damage something, causing you to start at the beginning trying to remember what you did. 

One caution.  A few minutes ago, I tried to download three libraries I don't already have and the procedure seemed to work well, with a window telling me I had succeeded and that I'd receive an email soon.  It hasn't arrived yet.  Emails usually arrive instantly.  Maybe Altium are more possessive of their treasure than they were some time ago.  I'll be patient and explore what I did wrong this time that I did right previously.

Good luck

Oh.

One more thought.

It is a bit misleading to think of the libraries with names beginning "Miscellaneous..." as "standard" libraries.  It is better to think of them as "quick and dirty" libraries thrown together to allow new customers to get started.  I think Altium are proud of their Vault, and I think they think of this as their "standard" library. 

The Vault probably works well for professional Altium customers designing the latest gizmo using the latest components, but it seems to have few leaded components, which I why I became so enthusiastic when I fount the cache of Unified Components.