Electronics > Altium Designer
Dangling wires
Gekofive:
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.
asmi:
Yes you can do that if required. There is a project setting "Net Identifier Scope" with the following options:
--- Quote ---
* Automatic (Based on project contents) – this mode automatically selects which of the net identifier modes to use based on the following criteria: if there are sheet entries on the top sheet, then Hierarchical is used; if there are no sheet entries, but there are ports present, then Flat is used; if there are no sheet entries and no ports, then Global is used.
The Automatic mode defaults to use the standard Hierarchical mode if need be, with power ports connecting globally. To use Strict Hierarchical, manually set the Net Identifier Scope accordingly. Hidden pins are always deemed to be global.
Flat (Only ports global) – ports connect globally across all sheets throughout the design. With this option, net labels are local to each sheet, i.e. they will not connect across sheets. All ports with the same name will be connected on all sheets. This option can be used for flat multi-sheet designs. It is not recommended for large designs as it can be difficult to trace a net through the sheets.
* Hierarchical (Sheet entry <-> port connections, power ports global) – connect vertically between a port and the matching sheet entry. This option makes inter-sheet connections only through sheet symbol entries and matching sub-sheet ports. It uses ports on sheets to take nets or buses up to sheet entries in corresponding sheet symbols on the parent sheet. Ports without a matching sheet entry will not be connected even if a port with the same name exists on another sheet. Net labels are local to each sheet, i.e. they will not connect across sheets. However, power ports are global – all power ports with the same name are connected throughout the entire design. This option can be used to create designs of any depth or hierarchy and allows a net to be traced throughout a design on the printed schematic.
* Strict Hierarchical (Sheet entry <-> port connections, power ports local) – this mode of connectivity behaves in the same way as the Hierarchical mode, with the difference being that power ports are kept local to each sheet, i.e. they will not connect across sheets to power ports of the same name.
* Global (Netlabels and ports global) – ports and net labels connect across all sheets throughout the design. With this option, all nets with the same net label will be connected together on all sheets. Also, all ports with the same name will be connected on all sheets. If a net connected to a port also has a net label, its net name will be the name of the net label. This option can also be used for flat multi-sheet designs, however, it is difficult to trace from one sheet to another since visually locating net names on the schematic is not always easy.
--- End quote ---
Gekofive:
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.
asmi:
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.
Gekofive:
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.
Navigation
[0] Message Index
[#] Next page
Go to full version