Circuit Studio realtime live help on Creating Libraries and Componets

Hi Stuart,

I am willing to help through this forum but not immediately available for hire as you suggest. Maybe someone else will take your offer.  Regardless, it may be helpful to continue a thread on library creation and maintenance.

Please put together a list of questions related to libraries that the forum can help with.  If they are detailed then make a new thread subject. Being in the forum helps others also.  I am always willing to learn from others suggestions.

Some general comments about libraries, for what its worth:

1) Look at Altium Designer related tech support videos and documents.  The libraries are compatible so some of the AD docs help.

2) I have found it simpler to NOT use the integrated libraries and keep my schematic and PCB libraries separate. Others may disagree.

3) Libraries are very custom to each users needs.  So, if I were to send you a library for schematic parts you probably don't want my parameters for part numbers.  I don't use the supplier links for pricing but others do.  It might depend on geography also.  You will need to link to specific footprints that you want. You need to figure out how you want to use these parameters and then build up your libraries.  Occasionally, I have had to go through my libraries and update all parts to add in parameters to all that I found useful.  Altium Designer is much more efficient with this since it has a spreadsheet view.  CS does not, and so it is a manual process.

4) For schematics, I separate parts into several library files.  Some are for connectors, another for resistors, another for capacitors, another for ICs.  As I build up more and more parts in libraries I may separate further into more files.

5) For schematic libraries, I use the same or similar text for Symbol Reference, Description and CompName.  In my case I put all resistors into a single library and have been building up separate parts for each value and package size.  Others may have separate libraries for each size (we did that at my previous employer with Altium Designer).

6) If using the Vault, I typically copy the part into a sandbox library, modify it to add in the parameters I care about and then copy it into my real libaries.

7) Schematic parameters at a minimum are probably the name, description, manufacturer, mfg part number, value.  That could build a basic BOM for a design.

8) Back up your libraries regularly!

9) For PCB libraries, I use a standard naming convention for IPC-7351.  You can web search for information.  Here is one link with an example: https://www.pcb-3d.com/tutorials/ipc-7351b-naming-convention-for-surface-mount-device-3d-models-and-footprints/

10) For PCB libraries, you will want to build up the layers to match how you work with PCBs.  That means, if you put courtyards on specific layer pairs then build libraries that way.  You may find that when you take footprints from other sources the layers don't match what you want and you have to move the layers.

Do you need an example set of libraries?  I could possibly post up a template of what I use as a starter.  Here is a screen shot of properties for a resistor.  I have worked with some people that wanted almost the entire datasheet worth of parameters and others that wanted as few parameters as possible.  Mine are in the middle.

Cheers.

Hi Thomas,

Thank you so much for your very detailed reply. That was very kind and considerate of you and I appreciate any help you can provide.  I'm sure I'm missing a single kernel of knowledge that stands in my way of grasping the CS library system.

I come from a long background of using OrCAD Designer and perhaps the CS nomenclature may be throwing me off.  For example, in OrCAD, I have created a number of custom component (Capture Library *.olb) libraries such as RF.olb, CAPS.olb, RF_PASIVE.olb and so on.  These *.olb libraries contain part "symbols" which are schematic drawings with part properties which I think are equivalent to the part symbols with properties contained within a CS *.SchLib library files.  Is that a valid statement?

Similarly, in OrCAD I have created custom footprints files such as CON_INCH.llb, RF_METRIC.llb, and so on.  These files contain PCB like footprints which look to be equivalent to the CS *.PcbLib files. Would you say that is also true?

OrCAD then takes the compiled net list which contains footprint and creates the PCB "Layout" *.max file.  Altium Designer and CS apparently hide that step in the Compile Document command in a *.SchDoc file.

The required footprint libraries have to be "Added" to the PCB layout.  I don't see a similar way of adding libraries in CS.

Let me continue by responding to your specific comments:

1. Yes, I have installed AD and reviewed the tutorials. AD seems very similar to CS and is helpful except with the bits I need for libraries.

2. I don't quite understand the integrated libraries, what benefit they offer, how to use them, and how to edit them. Its seems I agree with you in that regard and using on the SchLib and PcbLib are very similar to what I'm use to.

3. I agree her too.  However it looks like I can duplicate parts using a copy-paste method. For example to make a 2.00k resistor I could copy an existing say 1.00k resistor and simply edit the new properties but I don't see how to rename the new resistor.  How do I rename or save as when I do a duplication of a component in SchLib?

4. We think a like on this too.

5. Agreed.

6. I will set aside the Vault for now.  I've used it on AD and it worked well.  In my CS it doesn't seem to work well.  For example, if I search: 1k 5% 0805, the returned parts are all type of components and none of them seem to match my criterion. Also, since I only work on our internal products, I don't often need to search for parts and mostly use parts that we keep in stock.

7. Got that part fine, and the Library Component Properties works well for me and is quite understandable.

8. Back up regularly...good idea yes.

9. Good recommendation.  Thanks for the reference.

10. I'm a bit lost on that statement.  OrCAD footprint libraries have the ability to use any and all the layers that the Layout uses.  The concept of courtyards is new to me and is maybe Altium specific.

Yes!  It would be great to see how you set your libraries up.  I would appreciate the ability to look at one or two of your.

Thanks you sir for your generous responses.  Look forward to your next comments here.

Stuart

Hi Stuart,

I will attempt to address the first part of your recent post.  It does sound that a CS schlib is equivalent to an OrCAD olb.  Likewise, the CS pcblib seems equivalent to the OrCAD llb.

For a PCB, you add libraries as described here; Libraries | Online Documentation for Altium Products This brings them into the search paths.  When you update the PCB from the schematic it will search through the enabled libraries and pick the footprints that match.  It will either update them or pull in new ones from the libraries as needed.  There are selection options on how it searches or if it is pulled from a specific library instead of search order.

One thing that is not obvious is how it links parts between schematic and PCB.  This is done through a unique ID code.  When the PCB is updated from the schematic it tries to synchronize parts based on a variety of factors including the reference designator.  Once it links it should assign a unique ID code to each and they will then be controlled that way.  These links sometimes break and need to be relinked.  There are some other threads and some guides on this process.

Compiling a schematic and update to the PCB are not exactly the same thing. First compile the schematic and then update the PCB.

For the second part here is what I can say:

Without getting too crazy with parts, I have attached a small library of miscellaneous parts for schematics.  You can see some of the parameters I might add.  You will need to pick your own depending on how you want to use them. So, if you want pricing for BOM you would add in the suppliers links that I don't use.  But I do use component links for datasheets and Octopart.

You found you can copy and paste parts between schematic libraries and also from a schematic to a schematic library.  To rename a part, rename its symbol reference text.  Highlighted below in the Library Link section.  This sets the name in the schematic library.  Sometimes you cannot see this if the window is small. You would need to used the scroll bar on the Properties section.

Most ECAD environments I have used, including Altium Designer, CircuitStudio, PADs and OrCAD, have multiple methods of doing the same thing.  If you have not tried it, I suggest using the search box in CS for help and for commands also.  For example, in addition to editing the Symbol Reference text that I mentioned above, instead you can type rename into the search box and it will allow you to get to a box to change the name (if you are in the schematic library).  This search is sensitive to what window you are in.  I find a lot of interesting things you can do that are not in the command tool bar by using this method.

And finally, for PCB layers, CS tends to want to use certain layers for specific things such as outline, assembly information, silkscreen, etc.  I generally use the defaults that it uses. I find a courtyard layer useful for keeping parts spaced apart.  IPC 7351 has some standard definitions on these.  You can choose to follow or not.  Some designers build this into the silkscreen.  I sometimes do boards that don't have that luxury if parts such as chip scale and 0201 cases are used.  Courtyards help me with placement in such cases.

https://www.ultralibrarian.com/resources/blog/2020/04/09/top-four-recommendations-for-component-courtyard-management-ulc…

Hi Stuart,

I will attempt to address the first part of your recent post.  It does sound that a CS schlib is equivalent to an OrCAD olb.  Likewise, the CS pcblib seems equivalent to the OrCAD llb.

For a PCB, you add libraries as described here; Libraries | Online Documentation for Altium Products This brings them into the search paths.  When you update the PCB from the schematic it will search through the enabled libraries and pick the footprints that match.  It will either update them or pull in new ones from the libraries as needed.  There are selection options on how it searches or if it is pulled from a specific library instead of search order.

One thing that is not obvious is how it links parts between schematic and PCB.  This is done through a unique ID code.  When the PCB is updated from the schematic it tries to synchronize parts based on a variety of factors including the reference designator.  Once it links it should assign a unique ID code to each and they will then be controlled that way.  These links sometimes break and need to be relinked.  There are some other threads and some guides on this process.

Compiling a schematic and update to the PCB are not exactly the same thing. First compile the schematic and then update the PCB.

For the second part here is what I can say:

Without getting too crazy with parts, I have attached a small library of miscellaneous parts for schematics.  You can see some of the parameters I might add.  You will need to pick your own depending on how you want to use them. So, if you want pricing for BOM you would add in the suppliers links that I don't use.  But I do use component links for datasheets and Octopart.

You found you can copy and paste parts between schematic libraries and also from a schematic to a schematic library.  To rename a part, rename its symbol reference text.  Highlighted below in the Library Link section.  This sets the name in the schematic library.  Sometimes you cannot see this if the window is small. You would need to used the scroll bar on the Properties section.

Most ECAD environments I have used, including Altium Designer, CircuitStudio, PADs and OrCAD, have multiple methods of doing the same thing.  If you have not tried it, I suggest using the search box in CS for help and for commands also.  For example, in addition to editing the Symbol Reference text that I mentioned above, instead you can type rename into the search box and it will allow you to get to a box to change the name (if you are in the schematic library).  This search is sensitive to what window you are in.  I find a lot of interesting things you can do that are not in the command tool bar by using this method.

And finally, for PCB layers, CS tends to want to use certain layers for specific things such as outline, assembly information, silkscreen, etc.  I generally use the defaults that it uses. I find a courtyard layer useful for keeping parts spaced apart.  IPC 7351 has some standard definitions on these.  You can choose to follow or not.  Some designers build this into the silkscreen.  I sometimes do boards that don't have that luxury if parts such as chip scale and 0201 cases are used.  Courtyards help me with placement in such cases.

https://www.ultralibrarian.com/resources/blog/2020/04/09/top-four-recommendations-for-component-courtyard-management-ulc…