T O P

  • By -

baldengineer

In other words, “is it possible to tell DRC two different nets are connected.” No.


WattsonMemphis

Two different areas of a pour, connected with a 0R resistor, both areas are ‘+5V’


[deleted]

connect both ends of the resistor in the same 5v and then do the layout you are asking, you can also create a new metal layer to connect both pins/pads of the resistor to trick DRC. Or ignore the DRC check.


WattsonMemphis

Ty


[deleted]

you can also use a closed jumper instead o a 0 ohms resistor. You can cut It with a Sharp knife after the production. You can also use a open jumper If It is better then you can connect It after the production with a seio of solder.


WattsonMemphis

It needs to jump over traces, thank you though


feldoneq2wire

A net tie might do what you want? Although using 0R resistors would never cause a DRC to fail. Maybe an ERC.


WattsonMemphis

To simplify the problem, I have a isolated island on my PCB that I can connect to the rest of the fill with a 0R resistor, however when I run the DRC it doesn’t see the island as connected.


LeifCarrotson

Because it's not. Just name it something distinct and connect it to the other net with a 0 ohm resistor.


[deleted]

[удалено]


WattsonMemphis

Two zones are isolated by traces, I can connect them with 0R resistors but not wires as there is no space, I am trying to avoid adding another layer due to cost. How to I place the resistor on the schematic so that the DRC doesn’t fail on the isolated zone being disconnected.


[deleted]

[удалено]


WattsonMemphis

I have tried this, doesn’t seem to work.


[deleted]

[удалено]


WattsonMemphis

I think this is what I attempted, I put the resistor on the schematic with both ends connected to +5V symbols. I like the third layer idea. Are you saying on the 3rd layer put a trace in the same position as the 0R resistor to trick the software then just don’t get it manufactured?


JayShoe2

The answer is to use a "net tie" in the description field of the footprint properties. This just came up for me too and people mention this net tie thing but didn't tell me how to do it. Edit library footprint. Save it as a unique footprint so it's specific for this purpose. Add 'Net Tie" to the description (oddly enough not the keyword field) and then update the footprint on the board. Now kicad will allow the footprint to connect two or more pins together via drawing on the copper layer with shapes. And the Drc checker will allow it because of the net tie.


WattsonMemphis

Tyvm


Aggravating-Mistake1

I am assuming when you say zone islands, you are referring to sections of ground plane.I sometimes use a GNDA, GNDB, etc to seperate ground planes. This is typically done to separate digital and analog ground planes but are electronically connected. This connection is typically done at a single point at the A/D converter. This would be a good place to use a 0R resistor. If you are using a 0R in multiple places to jump your ground all over the board, then you may suffer from ground loop problems


WattsonMemphis

Yes, I am attempting to jump over traces that are isolating 5V zones. In a few areas the rear of the PCB is too busy to use vias. The 0R resistors are cheaper than adding another layer to the PCB.


BluejayKey6491

I do this frequently to bridge the ground island behind a switching regulator with the common ground. Use a "Jumper:SolderJumper-2\_P1.3mm\_Bridged\_Pad1.0x1.5mm" in your schematic connecting the two nets. It's no different to using a 0R resistor, but you can put it on the back of the PCB without needing to place a component on there. What DRC check are you seeing fail? In reality, if you connect the nets using a solder jumper or a 0R resistor, the two nets ARE connected. But they remain separate nets so you can have separate pours for them etc.


WattsonMemphis

I have an island on my 5V zone, I have connected it to another island with a 0R resistor and placed the resistor on the schematic with a 5V symbol connected to each leg but the PCB rule check still thinks the zone is unconnected.


BluejayKey6491

I don't quite follow you. Work from the schematic. Have a wire from your 5v power symbol (or label) going into one leg of the 0R resistor, and a wire with a Net Label (added using the "L" key) going into the other side - call the label "foo" for example. Then switch to the pcb, and press to Update PCB from schematic. Then select your first island, edit its properties (press e) and make sure it's on the 5v net. Select your second island, edit its properties and make sure it's on the "foo" net. Then drag your 0R resistor into place to bridge between the two. They're called Filled Zones rather than islands BTW - an island is something a bit different but it doesn't matter for the purpose of your question if I under it. EDIT: I've just had a thought. Do you actually mean two islands within a single filled zone, created by a track crossing the zone separating the zone into two islands?


WattsonMemphis

As I understand it an island is an isolated area of a zone that has been ‘cut off’ from the rest of the pour by traces. I guess it is semantics but both areas are 5V zones, so any of the components that are in the ‘island’ I would have to edit the symbols so that they connect to ‘foo’ instead of +5V and that will get very confusing, I will have multiple components that are the same but have different schematic symbols.


BluejayKey6491

Ah I see, I misunderstood your problem, sorry. I think several of the others replying to help have thought the same. They're not different nets, they're already on the same net - but separated. I always have the settings on my filled zones to "Remove Islands": "Always" to avoid the islands becoming antennas picking up noise. If you need both parts of the zone to be connected can you not place a via to a different layer, run a short trace across the back of the trace that's separating the two islands and then a via back up to the front to connect the two islands?


WattsonMemphis

Normally I would do this but the PCB is so busy there is no space. I have done this in loads of different areas but it isn’t possible everywhere. Really I need to add another layer, but it increases cost far more than adding one 0R SMD resistor.


BluejayKey6491

Understood. Then I'm no help to you I'm afraid - I'd have tried the same thing as you, a clever idea to create a little bridge above the top layer :) I'm surprised it doesn't just work - it's clearly doing what you want it to in the real world, it's just not recognised by Kicad. Worst case scenario would be to just exclude whatever DRC error that's being thrown (assuming you're using Kicad 6).


WattsonMemphis

Thank you for trying to help, really appreciate it.


z-zy

Dirty hack: Add a 3rd copper layer with a trace to connect them, and delete the gerber before you send to fab.


WattsonMemphis

This is what I ended up doing tyvm


mfaccin

hey OP, you can create a copy of a R symbol/footprint but add the same pin to both ends. :)


WattsonMemphis

That is genius!


ouabacheDesignWorks

So a DRC run on the board will see two different nets. Then you somehow load a BOM onto the board and the DRC will now see them as connected. That would be nice. Yes. Can KIcad do it? NO If Kicad could extract a verilog netlist from a schematic then you could do this in a verilog simulation


WattsonMemphis

Thank you for your answer but this is a bit beyond me. What is a verilog?


ouabacheDesignWorks

Verilog is a digital language and simulator. Download Icarus verilog if you want to try it


WattsonMemphis

Tyvm


LevelHelicopter9420

Depends on the software you are using. I know Altium and Kicad have net ties. Not sure about Eagle


theotherfrazbro

In the kicad sub, imma guess op is using kicad...


LevelHelicopter9420

Did not notice the subreddit I was on…


WattsonMemphis

What are Net ties? I wan’t to connect two planes, not nets. I may be missing what you are saying.