Dangling wires - Page 1
Forum section: electronics / general

author: Gekofive
author_rank: Newbie
timestamp: April 23, 2025, 10:13:17 am
content: In AD schematics, it is possible to have dangling wires considered to be connected together by just the net name.In other CAE apps, this is forbidden, and flagged by DRC (use of ports is mandatory even within the same page).Coming from one of those CAE apps, and possibly needing to switch to AD, I’m wondering if it is possible to set AD to work that stricter way.

author: asmi
author_rank: Super Contributor
timestamp: April 23, 2025, 03:13:36 pm
content: Yes you can do that if required. There is a project setting "Net Identifier Scope" with the following options:Quote

author: Gekofive
author_rank: Newbie
timestamp: April 23, 2025, 04:11:26 pm
content: Thanks @asmi for your answer.I'm not sure one of the options is the one I'm looking for.I'm totally new to AD, so it's not easy to explain using the right terminology specific to this app, but I try.Here what we'd need:1. all the connections have to be done using ports. No connection has to be permitted if based on "net label" only;2. all the dangling wires (with or without net labels) have to be flagged by DRC;3. no difference if single page design, multi-page flat design, or hierarchical design;4. global signals (i.e. ground) have to be listed somewhere and shares the same net label (i.e. GND) and the same symbol (i.e. ┴);5. if in the list, global signals are connected together on the whole design;6. if a net with a global signal net label (i.e. GND) is connected to the wrong symbol (i.e. VCC symbol), then DRC has to flag it;For the ones who know it, this is the behavior of Siemens xpedition CAE.I'm trying to make a plan of the troubles in porting a 30 year old company design procedures to a new CAE, so I do need support from experienced users (I can't learn to use a new CAE, just to check if it is acceptable or not... need a first evaluation before spending time on it).Thanks in advance for the help you can give me.

author: asmi
author_rank: Super Contributor
timestamp: April 23, 2025, 06:58:48 pm
content: 1. What is your definition of "dangling wires"?2. What's the use of net labels if not to connect pieces of the same net on a page without having to draw actual full wires (which will turn any somewhat complex design in unreadable spaghetti mess in no time flat)?Ports are only used to connect nets on different pages, while net labels are used to connect parts of the same net on a page (note that port does not automatically connect to a net with the same name as a port, and conversely, port can be connected to a local net with name different than that of a port itself - though utility of the latter is rather debatable). And it's not just AD's behavior, but also all other eCADs I've ever used, including Orcad Capture, DipTrace, KiCAD, EagleCAD.

author: Gekofive
author_rank: Newbie
timestamp: April 23, 2025, 08:10:59 pm
content: First of all, it is important to point out I’m not saying our way to work is the right one, and the others are not. My job is to evaluate if AD is a valid replacement for the eCAD used by a well-established company, using a different one from 30 years and having an equivalent well-established design protocol. The goal is to have the switch with the minimum impact on this protocol.With my surprise, the PCB placing and routing is not so demanding (in terms of procedures) as they are schematic entry and library management.Answering your questions:1. Dangling wires are the ones having one or both ends not (graphically) connected to a symbol. In Fig.1 you can see an example of dangling wire. As you can see, the DRC highlights (red star) the not connected end. It doesn’t matter if the wire is “named” or not, dangling ends are forbidden.2. Naming a wire has multiple functions.a. First of all, it gives a meaning to the circuit node. In Fig.2 you can see a wire (FSIN2) connecting several components. It is not connected to other parts of the schematics, but its name has a well-defined meaning. That signal (part of a measuring instrument) has accuracy constraints and on the internal product documentation is used on mathematical expressions.b. The wire name (net name) is visible on the routing procedure and it is very important for nets requiring special routing care.c. They are used on BUSes where wires enter and exit buses.In Fig.2 you can see even the net VM. It has an “inter-page” output connector mating with an inter-page input connector, in a different part of the schematic on the same page. The net starting from this connector has the same VM name. This “soft” connection works only because there are the two inter-page connectors; if you remove them, then you get a DRC error. This is the issue with AD, because it permits the soft connection even without inter-page connectors.

author: Someone
author_rank: Super Contributor
timestamp: April 23, 2025, 10:49:02 pm
content: This is enforced in the Connection Matrix, in combination with the above Net Identifier Scope.

author: Gekofive
author_rank: Newbie
timestamp: April 24, 2025, 05:59:17 am
content: Thanks @Someone for your reply.Please, let me better understand: do you mean it is possible to get what I need?In this case I can spend some time trying.

author: Gekofive
author_rank: Newbie
timestamp: April 24, 2025, 08:05:53 am
content: I checked the Connection Matrix, but it seems is not going to solve the problem.It rules the behavior of pins, not wires.In example, an output pin has not to generate error if left floating, but should do it, if a wire is attached to that pin and then left dangling.This seems not to be possible, using that table.The other important issue is the automatic "soft" connection of wires within the same page. A more direct question is:"Is it possible to generate a DRC error if, inside the same page, two separate wires share the same net label?"A related question:"Is there a "global nets" list as part of the project?"

author: Gekofive
author_rank: Newbie
timestamp: April 24, 2025, 08:37:58 am
content: Update:it seem there are both the DRC errors I'm searching for:1. "Duplicate Nets"https://www.altium.com/documentation/altium-designer/design-validation#duplicate_nets2. "Nets with only one Pin"https://www.altium.com/documentation/altium-designer/design-validation#violations-associated-with-nets(even if this one is not exactly what I'd like, but anyway acceptable)Now I can't understand how these errors are compatible with the real behavior of the schematic entry: almost all schematic examples have different nets connected to only one pin and sharing the same net name (soft connections)...Do these checking have to be enabled somewhere?

author: asmi
author_rank: Super Contributor
timestamp: April 24, 2025, 01:05:56 pm
content: Quote from: Gekofive on April 24, 2025, 08:05:53 amAll wires on the same page with the same net label are considered to be parts of the same net. This is super useful in complex designs to prevent schematics from turning into spaghetti of lines. I don't think there is a way to change that behavior.Quote from: Gekofive on April 24, 2025, 08:05:53 amNot that I know of. Depending on a setting I mentioned in my first response, some nets are automatically promoted to global nets, but I don't think there is a dedicated list of them anywhere.

author: Gekofive
author_rank: Newbie
timestamp: April 24, 2025, 01:56:00 pm
content: If two nets with the same net-name on the same page are seen as a single net, while two nets with the same net-name on different pages are seen as different signals, when the "duplicate Net" error is flagged?

author: asmi
author_rank: Super Contributor
timestamp: April 24, 2025, 03:35:48 pm
content: Quote from: Gekofive on April 24, 2025, 01:56:00 pmThe latter of those cases is going to flag an error if nets are not all made global, and setting, which makes local net names unique by adding a sheet number, is turned off.