Organize passive components Library in Altium

[Nikos A.]

Hi everyone,

Do you have any advice regarding organizing the library for passive SMD components (resistor,capacitor, inductors)?

Regarding the schematic the things are simple. One generic schematic for resistors and inductors, and two schematics for capacitors (polarized and non polarized)

The things are getting very messy with footprints. It doesn't make sense to me to have a single symbol for every part number that will return into a huge volume library with many identical footprints.

There are different sizes (0402, 0603, 1005 etc) and for each size there are 3 x footprints based on the IPC7351 (M,N,L)
Also the 3D model varies from manufacturer to manufacturer

My considerations so far:

- After some searching I decided to adopt the IPC Nominal Material Density
- Keep the same footprint for resistors, capacitors and inductors. For example, one footprint for 0603 for RCL components
- Use a universal 3D model for every category? I do not know..
- These components within the library will be in generic form, meaning they have no manufacturer part number associated with the footprint. When they are placed inside the design they will be assigned the supplier link and parameter (there is a great tool in Altium for this)

My goal is to maintain as few footprints as possible. How do you handle and organize you libraries regarding RCL SMD components?

Thanks

[tszaboo]

For example resistors: I've selected a large brand or resistors, that is usually on stock with all the values. Panasonic ERA is a good example, but I have a different range.
Made an excel sheet of all the values, description, manufacturer number, odercode. I organize it based on package size, order it on value.
Made a database library from this. Assign footprint and schematic designator for it.
I dont even think when I am designing something, just select it from the library. I also only have 1 footprint for 0402 0603 0805 etc.

Capacitors are similar. I have a range for fuses, precision resistors, power resistors, TVS diodes etc.

I know it is very hard to just abandon the old library, but that's what I did 5 years ago, and I am glad that I did.

[Nikos A.]

Thank for your answer @tszaboo

I dont even think when I am designing something, just select it from the library. I also only have 1 footprint for 0402 0603 0805 etc.

I like your approach, I am considering also keeping one footprint for 0402 0603 0805. What density level for the footprint design you're using?

Made a database library from this. Assign footprint and schematic designator for it.

So for every single componenent you have assigned a schematic and footprint? I was thinking to create a generic symbol schematic and a single footprint for every smd size and then assigning the parameters (part number, values and other technical details) during designing. Altium has the manufacture part search tool where you can assign manufacturer part parameters to any component that is placed on your design in seconds.

[voltsandjolts]

Here is my library of common Yageo 805 and 603 caps / resistors which all have Farnell and Digi-Key order codes:
https://www.eevblog.com/forum/altium/altium-standard-resistors-capacitors-and-inductors/msg840139/#msg840139

[voltsandjolts]

Made an excel sheet of all the values, description, manufacturer number, odercode.
I organize it based on package size, order it on value.
Made a database library from this. Assign footprint and schematic designator for it.

I need to try this.
Can you post the first few lines of the excel sheet, just to show the format?

[Nikos A.]

Here is my library of common Yageo 805 and 603 caps / resistors which all have Farnell and Digi-Key order codes:
https://www.eevblog.com/forum/altium/altium-standard-resistors-capacitors-and-inductors/msg840139/#msg840139

Thank you for sharing your library, really well structured!! I think I will go with this approach as well but I will keep in seperate libraries the res from caps.
So, every time you're inserting a new component you're checking that is compatible with you defined footprints right?
You have adopted your own footprint naming convention right? I mean you didn't follow the IPC standard..
What about the 3D models? You have a generic model for all res and caps?

Made an excel sheet of all the values, description, manufacturer number, odercode. I organize it based on package size, order it on value.
Made a database library from this. Assign footprint and schematic designator for it.

From your experience what are the advantages of using a database? Isn't more convenient to use manufacturer part search and add the parameters automatecally?

[tszaboo]

Library Ref   Footprint Ref   DESCIPTION   MANUF   MANUFCODE   DIGIKEY   FARNELL   SMD   VALUE   NoPins   SUPPLY   VOLTAGE   TECH
CAP   CAPC1206N   CAP CER 10PF 1KV X7R 1206   AVX   1206AC100KAT1A   1206AC100KAT1A-ND      YES   10pF   2   SUB   1000   X7R
CAP   CAPC1206N   CAP CER 10PF 1KV NP0 1206   AVX   1206AA100KAT1A   1206AA100KAT1A-ND      YES   10pF   2   SUB   1000   C0G, NP0

Tabulations might show wrong on the forum.
This is the first two lines of a library containing KV rated MLCCs. Library Ref points to the schematic symbol, footprint ref points to the footprint. I only have 1 SCH symbol and maybe 5 Footprint for this library.

From your experience what are the advantages of using a database? Isn't more convenient to use manufacturer part search and add the parameters automatecally?

No, I dont think it is. I have all the Resistor and capacitor values I would ever need, the footprint is tested, and I dont need to change anything to create the BOM in the format I would like it. OK, maybe 1-2 things, some library I mark SMD as yes, some as TRUE. And there is a tiny bit of inconsistency between libraries so there is a bit of copy paste on the SCHlib list.

I just dowloaded a few components from the cloud. It had text on Mechnical layer 1, and I almost didn't catch it. Layer 1 is the outline for me, and that gets added to every layer. So this text almost ended up shorting tracks on all 4 copper layers.

[cortex_m0]

What about the 3D models? You have a generic model for all res and caps?

For passives, the 3D model isn't super important. It's very rare (teetering on never) that I have a design where the height of an MLCC or resistor is relevant. So even though there are low-profile caps on the market, assuming the largest 1206/0805/... is sufficient.

That may change if you're Samsung trying to squeeze every 0.1mm of thickness out of a phone.

From your experience what are the advantages of using a database? Isn't more convenient to use manufacturer part search and add the parameters automatecally?

There's a dividing line between hobbyists and professionals here IMO. If you're a hobbyist, there's no problem with entering the part numbers and parameters manually. But if you're a company, it's helpful to not have to do that repeatedly. My company uses a database, and so the last time someone had to think about the 10.0K 0603 1% resistor was 20 years ago. Now we just pick it and have a high degree of confidence we'll get the right part placed. The only problems occur when purchasing says that part number is in short supply.

[Nikos A.]

Thank you all guys!!! Very helpfull your input!!

[Ice-Tea]

My own 0,02$: use a different 3D footprint for caps and resistors (at least the color). It helps a lot to make a 3D view of the board more "obvious".

[voltsandjolts]

Here is my library of common Yageo 805 and 603 caps / resistors which all have Farnell and Digi-Key order codes:
https://www.eevblog.com/forum/altium/altium-standard-resistors-capacitors-and-inductors/msg840139/#msg840139

Thank you for sharing your library, really well structured!! I think I will go with this approach as well but I will keep in seperate libraries the res from caps.
So, every time you're inserting a new component you're checking that is compatible with you defined footprints right?
You have adopted your own footprint naming convention right? I mean you didn't follow the IPC standard..

That handful of footprints have generic names rather than IPC names and that is deliberate.
IPC names are quite descriptive, so you can't change the footprint much or the name becomes incorrect.
So you basically have to create a new footprint, then update your whole library with the new footprint IPC name.
Not an issue with Altium Designer but a huge PITA in Altium Circuit Studio (which I was using when creating the library).
So I used generic names to allow for lazy footprint changes.

What about the 3D models? You have a generic model for all res and caps?

I wouldn't recommend a different 3D model for each resistance of resistor 

[hsn93]

just worth sharing here..

https://youtu.be/fRaPwBUokJQ?t=261