| Author |
 Topic  |
|
|
cioma
125 Posts |
 Posted - 06 Jul 2016 : 15:20:29
|
| I'd like to mark a functional pin of a component in schematic as "No Connect" so ERC would know is was intentionally left unconnected (ERC rule "Pin Not On A Net Error"). Is there a way to do it in Pulsonix? E.g. some other ECAD tools have a special "No Connect" symbol. |
|
|
steve
United Kingdom
316 Posts |
Posted - 06 Jul 2016 : 16:04:05
|
There is a 'No Connect' Pin Type within the choices for a pin in the mapping of a Part. Please see Help - Technology - Pin Type Names.
Pulsonix Assistance |
 |
|
|
cioma
125 Posts |
Posted - 07 Jul 2016 : 09:53:30
|
Well, I don't need to have a part pin to have a pin type of "No Connect", I need to mark a pin on a component in particular schematic as no connect so Electrical Rules Check doesn't flag an error.
For example, there is a configuration pin on a certain component that, depending on application, needs to be either connected to ground or left unconnected. In part definition this pin type shall be "Input". Then I use this component in a schematic that requires this pin to be left unconnected. When I run ERC on such schematic it gives me an error (as from the formal standpoint an input pin is not connected to any net). So I'd like to somehow tell ERC that this pin was left unconnected intentionally. Thus my question: does Pulsonix currently allow doing that? |
|
|
|
steve
United Kingdom
316 Posts |
Posted - 07 Jul 2016 : 11:35:51
|
In this example, after running DRC with that check set on, you would lock that error. This is normally used to mark an error which the designer considers to be acceptable and which does not need checking again.
Pulsonix Assistance |
|
|
|
hippenstiel
Germany
15 Posts |
Posted - 07 Jul 2016 : 14:04:23
|
You could also leave the Pin Type as Input in the library and override the pin type to "No Connect" locally in the design. Go to the properties of the pin. Check the Override checkbox for Pin Type and select No Connect.
It has the advantage over the locked error, that it stays, even if you move the component again. |
|
|
|
cioma
125 Posts |
Posted - 07 Jul 2016 : 14:32:47
|
Thanks for both solutions, I'll use them depending on particular situation.
I think it still would be useful to have a "No Connect" documentation symbol in Pulsonix. Perhaps is could be considered for a future release? |
|
|
|
cioma
125 Posts |
Posted - 24 Jan 2017 : 10:48:03
|
Could this suggestion be filed in Pulsonix bugtracker?
I've just done ERC on a design with a couple of hundred intentionally unconnected pins and it's a nightmare to lock the errors as one needs to double-click on an error to see if related pin was left unconnected intentionally or not. |
|
|
|
jameshead
United Kingdom
125 Posts |
Posted - 24 Jan 2017 : 11:02:15
|
quote:
I've just done ERC on a design with a couple of hundred intentionally unconnected pins and it's a nightmare to lock the errors as one needs to double-click on an error to see if related pin was left unconnected intentionally or not.
My view is that this is exactly what the designer must do: to go through every error flagged up by the ERC check and determine if it's an intentional error or something "not-quite-right".
If you have a component such as a microcontroller or a microprocessor that's going to have many unconnected pins then the previous advice is appropriate. The designer should select the unused pins in the schematic (which can be done many at a time), right-click, select properties, and change the pin type to unconnected.
There's also a chance at this stage to change the pin style to a different style to make it obvious in the schematic and print out that the pin is intentionally unconnected.
I use a pin style called "Pin Not Connected" that's a filled in square, that's set up in my schematic technology file. Just tick the box next to Pin Style and select the pin style you create for an intentional unconnected pin. |
|
|
|
cioma
125 Posts |
Posted - 24 Jan 2017 : 17:26:00
|
| I prefer not to change library-related properties (e.g. pin types) on a component instance in schematic to make sure all parts in schematic are exactly as in library. Besides clicking on pins and changing pintype for hundreds of pins is laborious and error-prone. Using a "No Connect" symbol is way more convenient and reliable. And when I put it on a pin I already explicitly say that it's intentionally unconnected ;) |
Edited by - cioma on 24 Jan 2017 17:26:40 |
|
|
| |
Topic |
|
