Assigning Design Item ID to Comment - Page 1
Forum section: electronics / general

author: qwerty18
author_rank: Newbie
timestamp: May 29, 2018, 06:17:50 pm
content: Hi everyone,does someone know a way to place a component with the Design Item ID as the Comment?It bugs me, that the default text under the symbol is always specified in the symbol itself.Since I am using a database library with some symbols linked to multiple footprints, i have to edit the comment manually after placement to reflect the manufacturing number.I'm happy for any suggestions

author: ajb
author_rank: Super Contributor
timestamp: May 29, 2018, 06:34:02 pm
content: In the SchLib you can set the value of a text string to "=ColumnName" (without the quotes). This works for the comment and should work for additional text strings that you place as well. Alternatively, once you place the symbol, you can use the properties window to make whichever database parameters you want visible on the sheet. You may also be able to add a parameter to the symbol in the schLib and link that to the database parameter so it shows up automatically, I haven't tried.Personally, I set the comment in all of my schLib symbols to "=Value", and then in my database the Value column is set to whatever is appropriate to the part--it might be "10k" for a resistor, or it might be a complete part number for a specific IC. I have a separate column for manufacturer/supplier PNs, and those are what get placed into the BOM. That keeps only essential design information in the schematic, but everything needed for manufacturing can easily be pulled out when needed.

author: qwerty18
author_rank: Newbie
timestamp: May 29, 2018, 07:56:53 pm
content: Setting the value with "=Part Number" works well.Since every part has already parameters from octopart, I am going to assign the comment directly to the relevant parameter, like "resistance".Anyway, thank you very much, you helped me a lot

author: julianhigginson
author_rank: Frequent Contributor
timestamp: May 31, 2018, 02:31:53 am
content: I'm with AJB, all schematic components get "=value" in the default comment field. then in the db, all components get the "value" field set to whatever is appropriate. then the description field just picks that up and shows it.for jellybean parts it's the resistance, capacitance, inductance, etc. Maybe sometimes also some secondary characteristic that's special about the part... like say, voltage of a polarised cap, or if it's low ESR or extended accuracy or something like that. (anything that's critical for the performance of the actual part in a specific schematic, I will put in nearby as a standalone text string)For an IC, it might be the base IC part number (ie missing any package definition)For a switch it might be a basic description "momentary tact" for example.Of course, the database also holds full manufacturer part number and manufacturer name and digikey-style part description fields amongst other things.

author: ajb
author_rank: Super Contributor
timestamp: May 31, 2018, 05:55:10 am
content: Quote from: qwerty18 on May 29, 2018, 07:56:53 pmA word of caution, having gone done this road myself--it's tempting to go crazy with your database structure and throw in columns for all kinds of different parameters, so that you have a ton of useful parametric information right in your part library, but this is ultimately a waste of time in my experience. You either have a ridiculous number of columns in one database table, or you have to have separate tables with different schemes for each class of part, and both quickly get unwieldy and difficult to maintain.Instead, just put in the primary value for the part, a human-readable description that captures key specs, and a link to the datasheet. For most jelly bean parts, all you need is that short description when picking something out from your library (and the description is especially helpful in BOMs, etc, because it immediately tells the reader what sort of thing it is without having to decipher a PN). For more complicated parts (ICs, even transistors and diodes in some cases) you will *never* be able to capture all of the factors that go into determining whether a particular part is fit for your purpose in a set of database fields anyway, and that's where the datasheet link comes in. If you follow Altium's field naming for it, it will even be available via right click in the schematic editor.For situations where you want a bit more info to appear on the schematic, you can add a couple of "special" fields to the database, and as long as your consistent in how you use them ("Special 1" is always tempco for resistors and dielectric for capacitors, etc) it's easy to create alternate schematic symbols that show those parameters automatically. That way your basic pullup resistors that don't really matter can just show a resistance, but for your analog section you can clearly specify where the special high precision $5/ea ones go.