Author Topic: Have a component on schematic that has just pins or headers for footprint  (Read 3704 times)

0 Members and 1 Guest are viewing this topic.

Offline TheUnnamedNewbieTopic starter

  • Super Contributor
  • ***
  • Posts: 1208
  • Country: 00
  • mmwave RFIC/antenna designer
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)
The best part about magic is when it stops being magic and becomes science instead

"There was no road, but the people walked on it, and the road came to be, and the people followed it, for the road took the path of least resistance"
 

Online ajb

  • Super Contributor
  • ***
  • Posts: 2582
  • Country: us
Re: Have a component on schematic that has just pins or headers for footprint
« Reply #1 on: September 22, 2017, 01:10:22 pm »
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 several component types that Altium provides:

Quote
Type Select one of the following component types from the drop-down list:
Standard - These components possess standard electrical properties, are always synchronized, and are the type most commonly used on a schematic sheet.
Mechanical - These components are not checked for electrical properties/errors or synchronized. This type is used to include additional mechanical objects, such as a mounting screw or a heatsink. They are included in the BOM.
Graphical - These components are not checked for electrical properties/errors or synchronized. This type is used for tasks such as adding a company logo to a document. They are not included in the BOM.
Tie Net (in BOM) - These components short two or more different nets and these components will appear in the BOM and are maintained during synchronization.
Tie Net - These components short two or more different nets and these components will NOT appear in the BOM and are maintained during synchronization.
Standard (No BOM) - These components possess standard electrical properties, and are synchronized BUT are not included in any BOM file produced from the file.
Jumper - These components are used to represent a wire link, typically used on a single-sided board. On the schematic, Jumper-type components do not need to be wired in, they are only included to ensure that the Jumpers get included in the BOM. On the PCB, set the jumper pads to share the same non-zero JumperID value; the software recognizes this state, adds a symbolic link between the jumper pads to represent the wire link, and factors the link into design rule checks.

If 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.
 

Offline T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 21606
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: Have a component on schematic that has just pins or headers for footprint
« Reply #2 on: September 22, 2017, 06:26:10 pm »
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
Seven Transistor Labs, LLC
Electronic design, from concept to prototype.
Bringing a project to life?  Send me a message!
 

Offline TheUnnamedNewbieTopic starter

  • Super Contributor
  • ***
  • Posts: 1208
  • Country: 00
  • mmwave RFIC/antenna designer
Re: Have a component on schematic that has just pins or headers for footprint
« Reply #3 on: September 23, 2017, 11:07:57 am »
The schematic symbol doesn't have to resemble the footprint, you can assign whatever footprint you want to a part. :)

Tim

Oh 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.
The best part about magic is when it stops being magic and becomes science instead

"There was no road, but the people walked on it, and the road came to be, and the people followed it, for the road took the path of least resistance"
 

Online ajb

  • Super Contributor
  • ***
  • Posts: 2582
  • Country: us
Re: Have a component on schematic that has just pins or headers for footprint
« Reply #4 on: September 23, 2017, 04:58:12 pm »
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.
 

Offline T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 21606
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: Have a component on schematic that has just pins or headers for footprint
« Reply #5 on: September 23, 2017, 07:04:25 pm »
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
Seven Transistor Labs, LLC
Electronic design, from concept to prototype.
Bringing a project to life?  Send me a message!
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf