The Jumper options seem to be limited to wire jumpers - vias and unlimited length wires. Is there a way to specify something like a 1206 (zero ohm) resistor as a jumper?
Since you want this part to appear in the BOM (as a POP or NOPOP), you must specify it in the schematic. ECOing parts in Layout is tricky. If you change the schematic later, the fudged part may disappear (depending how you added it in manually).
You can see how I do it in this post:
Thank you for the link but has there really been no update to this functionality in PADS itself in all this time? I imagined something along the line of a "bridge" designator in Logic or Layout but I guess I'm just dreaming!
Another question: You have the jumper part with two pads and associated copper. You connect two separate nets to each pad but have them connected in the part. How do you handle this if you want not two separate nets but the same net. For example, I want to jump +5 across certain spots on a board that cannot have non-GND vias. I would like to be able to add 3 or 4 of these to the schematic and place them in areas where single layer routes are becoming isolated from their destination. Have you done this in the past?
They do have a bridge component now but I'm not a fan, so I don't recommend it in posts.
It sounds like you have unroutable nets that you want to manually jump after the board is made. I think you have a routing problem, not a part problem. That's why PADs does not allow you to do what you want. If you really want to go this way, break the net into subnets with slghtly different names, then add zero ohm resistors.
That's easy to say... this happens on TClad boards (mostly used for power) and in RF designs with one copper layer, no vias or other routing layers available. I want to be able to drop a jumper as I am routing those types of boards. Currently I have to go back to the schematic and add the jumper, then ECO to layout. but then maybe I won't really like that route, and I'll need to go back and change it again. Since jumpers are supported, it seems like it would be nice to take the next logical step and all me to specify some other footprint for the jumper.
It does seem like it's a next logical step to add this feature. Either by incorporating it into the jumper feature or just making a two pad via that routes through an "air" layer. Anyway, the suggestions in the thread have been very helpful but I decided to basically use an 0603 PCB decal with a part number that has the ref designator of JUM. I place the same net on both sides but protect the connection between them while routing. This way, I have a number of unroutes, like so:
This way, my connectivity errors are limited to "isolated subnets" or something to that effect. I just confirm that each of those errors contains at least 1 pin that has a JUM designator and move on.
You are very correct, though, that it is a pain to work around. It involves more manual routing on lines that I would usually designate as "don't care" and do autoroute. It also involves, as you said, going back into logic and adding these jumpers.
To say that there are no uses for this functionality is silly. My board needs to be no more than 2 layers and cannot have vias. Anyway, I hope my input helps (or at least helps you decide what NOT to do!).
Retrieving data ...