I'm having a hard time working with Altium's BOM management - here's my issue: I'm using general components like the shown 0402 capacitor part used in hundreds of places across the schematic. In these, there are issues with individual parameters (incomplete description, etc) on some of these parts. Ideally I'd like to group these parts together and update their parameters together, because it would literally take a week of copying and pasting to do this one by one with the schematic sheet.

The ActiveBOM seems like a good way to organize this, but I'm running into problems. I cannot seem to update any of the parameters in the parts listed without finding each one in the schematic. In the screenshot shown below, some of the descriptions of the same type of part are incomplete and show up as different parts entirely, despite being grouped by part number.

I clearly am working in a way that Altium has not intended. Can anybody point me in the right direction for cleaning up my BOM?

ActiveBOM screenshot

  • \$\begingroup\$ I take it you don't want to/can't smart search and update from the properties tab? \$\endgroup\$
    – vir
    Commented Feb 15, 2023 at 20:56
  • \$\begingroup\$ Just read up on this feature. A bit more clunky than I was imagining, but this definitely works. Thank you for the suggestion! \$\endgroup\$
    – ethan
    Commented Feb 15, 2023 at 21:02
  • \$\begingroup\$ It appears that this only works within the open schematic sheet...better than nothing, but still seems like there must be a better way \$\endgroup\$
    – ethan
    Commented Feb 15, 2023 at 21:23
  • 1
    \$\begingroup\$ The last time I checked, "Parameter Manager" allows you to modify component parameters all at once. Also makes it easy to find those pesky parts that are slightly different, and fix them too. (schematic Menu bar) \$\endgroup\$ Commented Feb 15, 2023 at 22:03
  • \$\begingroup\$ Aha! This looks promising. I knew there would be something silly I was missing. \$\endgroup\$
    – ethan
    Commented Feb 15, 2023 at 22:06

1 Answer 1


Look in to using the Update Parameters From Database (found in the tools menu, keyboard shortcut T D) which is equivalent to Orcad's Include file technique. This requires Microsoft Office to be installed. If you don't have Office installed, then install the Microsoft Access Database Engine Redistributable. This technique is fine for individuals, but much harder to maintain for many users. Refer to Altium's online manuals to implement this.

You create an Excel database file with the parts you are using. Altium will field match certain fields like library reference and value and stuff the parameters of your choice (perhaps footprint, description, manufacturer part number, manufacturer, and your company part number) to each schematic part.

An example of an Excel spreadsheet.
Library reference and value are part of the component parameters in your schematic that you entered.
The rest of the items (footprint, description, Mfgr_pn, Manufacturer, Company_pn) are stuffed in to the matching parts using the Update Parameters from Database tool.

\begin{array} {|r|r|}\hline Library Reference & Value & Footprint & Description & Mfg\_PN & Manufacturer & Company\_PN \\ \hline R0402 & 10.0 & R0402 & RESISTOR, 10.0, 1\% & ERJ2RKF10R0X & PANASONIC & 110010R0 \\ \hline LT3094 & LT3094 & LCC12.3X3mm & NEG \;REGULATOR & LT3094EDD & ANALOG DEVICES & 22000124 \\ \hline \end{array}


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.