Net Ties - Page 1
Forum section: electronics / general

author: generic_username
author_rank: Regular Contributor
timestamp: October 02, 2019, 11:01:49 am
content: Hello everyone.In the past when connecting 2 different named nets I used a 0 Ohm resistor as a connection point.Today I found out there's net ties for that purpose.So I have a rather odd question as I'm arguing with my collegue about this feature.Why create an extra part when you can just connect two nets in the PCB layout together and create a rule that allows short circuits?(well apart from the obvious reason that the DRC can't detect if you mess up and have multiple connections instead of just 1)kind regards

author: Andy Watson
author_rank: Super Contributor
timestamp: October 02, 2019, 11:25:08 am
content: Grounds and other common rails (I would guess). Having the same net name is useful for automatically connecting nets - such as when pouring ground planes. Having a dedicated component - i.e. a zero-ohm link - allows it to be placed automatically at assembly time, and it puts it on the BOM.

author: enz
author_rank: Regular Contributor
timestamp: October 02, 2019, 11:29:11 am
content: Quote from: generic_username on October 02, 2019, 11:01:49 amBecause then you don't have a chance to control how and where those two nets are connected.One of the reasons you need something like a net tie is because you want to connect two nets only at a certain point of the PCB (and only there).If you create a DRC rule to allow short circuits, you wan't be able to catch any accidental short circuits elsewhere on the PCB.Martin

author: Pseudobyte
author_rank: Frequent Contributor
timestamp: October 02, 2019, 03:31:18 pm
content: Exactly what enz said. It is fairly common, especially in high power motor controllers to have separate digital and power ground planes. We use small board features in the form of a footprint to join the two ground planes in one place that is carefully decided. We do this to control the return paths of each circuit section. You can't just leave them isolated because that would create loads of other problems, so we tie them together for that galvanic connection. In this case the net tie is just to make them the same potential. Not designed to carry current (exactly what we are trying to prevent).

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 03, 2019, 03:49:30 pm
content: How-to is covered in Altium's guides. Basically draw a footprint with two pads (remember to remove soldermask and paste openings*) and a trace or Region between them, and set the component type to Net Tie (BOM or non-, as you prefer). That suppresses DRC errors on the shorting copper.*Unless you want to use it as an optional jumper, in which case make, say, a resistor footprint with a shorting trace between pads. That way you can place a resistor if you ever want to re-jump it, without having to scrape and tin anything.Net ties can get you different rules for local sub-nets, handy for autorouting. Be very weary of using them for grounds or other large connections, and be very weary of connecting anything between domains so divided. This goes exactly the same for any large nets that have been slotted -- sometimes, you'll slot ground to help isolate noise, but this is only to be done with careful consideration. In particular, do not cross traces over slots, at least without a lot of filtering. The same goes for net ties.I've seen them abused, where it was seemingly thought that throwing net ties everywhere magically isolated the circuits; except they were done irresponsibly, and even within that idea, there were blatant loops shorting around the ties. That was a doubly-wrong design...I've also seen them used where the voltage drop is assumed to be zero, so that for example a current-sense resistor on the power plane was sensed by a comparator on the digital plane. It's not obvious if that comparator will behave, or generate gibberish on every switching edge.Avoid these pitfalls, and you will probably find it's very rare that you need a net tie, but on the odd occasion when you do, they are indeed handy.Note that you don't need to make a net tie narrow (like a resistor), or on the outside only (you can put the copper on an inner layer; you can also set the component itself to an inner layer, but this may generate confusion in the fab outputs, because boards can actually be fabbed with embedded components -- this is just FYI in case anyone asks, just explain it's a copper feature only), you can make them in whatever shape you like. A wide tie may be effective for local planes; multiple can even be used in parallel to extend the perimeter in contact, or a corner or other oddly shaped tie can be made to fit in just the right place. An annular ring net tie can be made to apply different rules to a local net, while fully surrounding and connecting that net. You can get quite creative, just keep in mind the work required to change it in the future, if it should ever be necessary.Tim

author: dmills
author_rank: Super Contributor
timestamp: October 05, 2019, 12:35:00 pm
content: One place I often use them is in audio designs where I want the two decoupling caps on the opamp supplys to be connected together and then that net connected to my reference at one point.This keeps the class B current switching pulses as the output stage changes quadrant away from the sensitive reference net. A PTH hole with a small pour on two different layers does quite nicely for this.They have their place, like everything else.Regards, Dan.

author: generic_username
author_rank: Regular Contributor
timestamp: October 09, 2019, 11:29:10 am
content: Thank you all for your comments , was fairly more than I anticipatedand sorry for late reply