Have a component on schematic that has just pins or headers for footprint - Page 1
Forum section: electronics / general

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: September 21, 2017, 08:38:06 am
content: On a design I'm working on, I have a torroid transformer with two output windings (2x12V). I would like to just have two connectors for each winding. Is there any way to tell Altium that this is an "off-board" device and have me just place headers as it's pins, without Either having to put in some kind of connector for each channel, or use multiple actual components to represent a single transformer?In other words: I have a device that does not have a fixed footprint (as it is just cables). How would I best design around this in Altium, as using a single footprint limits my freedom of placing the different connectors wherever I would like them (with respect to eachother)

author: ajb
author_rank: Super Contributor
timestamp: September 22, 2017, 01:10:22 pm
content: If you're asking how to have one schematic symbol that results in two different parts on the PCB, there's no way to do that in Altium.If you want a symbol in the schematic for the transformer, but don't want to have that put a component on the PCB, then you can create a "Graphical" component for it. This is one of severalcomponent typesthat Altium provides:QuoteIf you want to show the transformer on the schematic and have individual componets that you can place for each of the winding connections, you probably want to use standard components for each of the winding connections, and use a graphical component for the transformer (or just draw the transformer directly in the schematic). If your winding connections will be just pads that wires get soldered to, then you can create "Standard (No BOM)" components for the pads. These will still get synchronized and be included in the netlist, but will not appear in the BOM (since there's no component to be purchased and fitted). Standard No BOM components are also useful for things like fiducial marks, solder jumpers, logos, etc.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 22, 2017, 06:26:10 pm
content: Want a header? Select a header footprint and match up the pins as needed. The schematic symbol doesn't have to resemble the footprint, you can assign whatever footprint you want to a part.Tim

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: September 23, 2017, 11:07:57 am
content: Quote from: T3sl4co1l on September 22, 2017, 06:26:10 pmOh ofcourse, but the thing is that here, my transformer might have multiple windings. To my knowledge - only one footprint can be attached, and it will fix the locations of the various cables with respect to one-and-other. But in this case, I am able to put each cable (almost) completely independent of the locations of the other cables. Hence, just selecting a header footprint and matching up footprints won't really work, I think.

author: ajb
author_rank: Super Contributor
timestamp: September 23, 2017, 04:58:12 pm
content: So just create a component for each of the connection you want to be able to place individually, and do whatever you need to do in the schematic to clarify your intent. See attachment. You can create a footprint that is simply a pad, as P1-3 are, and link it to an appropriate schematic symbol. Place them on the schematic however suits your design, and you can even doodle some wires and some wire-mounted terminals to show how the off-board wiring will be done. Or you can place single-wire connectors, like T1-3 (which are PC-mount QC terminals), if that's what you want. The transformer can be done as different sorts of components depending on whether you want it to appear on the PCB and/or in the BOM.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 23, 2017, 07:04:25 pm
content: Ah yes, I've done that before,This was a transmission line transformer. I wanted two header footprints, for various reasons. The ferrite core sits between the headers: I used some graphics to imply this. In this case, a full footprint would've been sufficient, but I wasn't going to do that for a one-off.Tim