6
\$\begingroup\$

How you deal with resistors and capacitors in Altium?

If you have a single resistor/capacitor, it is easy later to change values, etc, but how do you deal with the BoM later?

But, if you have different components, i think it is a nightmare!! there are so many!! with links, etc. And I think, you have the same problem here, because for a resistor, there are many supplier id's...

How do you manage all this?

\$\endgroup\$

6 Answers 6

5
\$\begingroup\$

We use multiple resistors, each with separate values in custom fields that we've added such as manufacturer info, etc. Takes time but in the long run it makes creating the BOM easy.

This means you can't readily just change the component value and you have to actually code the part.

\$\endgroup\$
2
\$\begingroup\$

Some people like to have the schematic fully specify everything, as Gustavo suggests. I preferred to keep the schematic simple, and manually edit the BOM to add supplier and part number information.

I used a BOM format that gathered all identical components together - one line might say "25 10K 1/4W resistor" - then I would add the supplier and part number to that line. If I had to change supplier, I only had one line to change, rather than all the parts on the schematic.

\$\endgroup\$
2
  • 2
    \$\begingroup\$ For small projects yes. But multiple projects where you want to reuse some elements this can become a bit of a nightmare. \$\endgroup\$ Commented Sep 13, 2013 at 17:13
  • 2
    \$\begingroup\$ @GustavoLitovsky: I suppose the method will depend on the work environment. Where I worked, I generally did the whole project, and rarely produced more than a dozen units of each design, so my method worked for me. In a larger company, with corporate-controlled purchasing and parts stocking, your method may be more appropriate. \$\endgroup\$ Commented Sep 13, 2013 at 17:50
2
\$\begingroup\$
  1. The best thing to do is to create all the standard footprints once. Put them in a mother Integrated Library.

  2. Once you're done with them, create another (read:project-specific) Integrated Library for each new project you begin.

  3. Then copy footprints/symbols as and when required from your mother Integrated Library and you are good to go.

  4. I'd recommend coding the part number into the symbol for each project specific library. When reusing the symbol, manually change the part number, if using a different part.

  5. It might seem like a lot of effort when making the library for the first time, but that will be pretty much the last time, at least for resistors and capacitors.

\$\endgroup\$
2
  • 3
    \$\begingroup\$ I usually use components from a central library while designing the circuit, and then use the "Create Library from Project"-function to build a library with the exact parts used in the project to be packaged with the project files. This way I can still edit/open/store the project as necessary without access to the central repo (if I send it out for QA, etc), and in the exact same state as it was when it was produced. Any flaws in footprints are fixed in the central repository, and then a new project library is generated when a new version of the board is made. \$\endgroup\$
    – Araho
    Commented Jun 14, 2017 at 10:41
  • \$\begingroup\$ @Araho: +1 for teaching me a new method. This process seems more neat than mine. \$\endgroup\$
    – Sachin
    Commented Jun 15, 2017 at 5:27
1
\$\begingroup\$

Single resistor for 0603, 0805, ... The comment field contains the article number from the ERP system and is entered manually. Yet, if you use a e.g. 0R resistor more often, you can simply Copy&Paste it in which case it will keep its fields.

The ERP also has a long text for that very part. So when the BOM is created, it will print out the long text as well.

\$\endgroup\$
1
\$\begingroup\$

For best design integrity, every component should map 1:1 to a real physical component, e.g. something you could order from Digikey or wherever. It's more work on the front end but much less work on the back end; you don't need to constantly verify the part numbers on your BOM. In reality, once you create a few of the basics like a 10k ohm 0603 resistor, then creating an 0603 resistor with a different value is a fairly simple copy-paste-modify operation. Nowadays I try to use the supplier links so that I can verify that my part number is indeed a real order able part.

Minor note: if you're creating a large component library then standardize. For example, all my generic resistors are 1%. This way we don't have some 5% parts and some 1% parts. Also be standard about custom parameters for each component. I use the following:

  • MF: the component manufacturer MFPN: manufacturer's part number ComponentLink1Description : this enables the 'reference' right click menu for the component. Usually this is 'Datasheet' ComponentLink1URL: the URL to the data sheet, for example.
\$\endgroup\$
1
\$\begingroup\$

My advice is to use a database library, even locally. In this way, only excel etc. you can easily create a library of all resistor values at once in the database. Then you can directly pull it out and use it or replace it.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.