as far as I know when you use "nets and ports global" it will connect up via net names in preference to using the port symbol. I think (but haven't checked) that if you have un-named nets connected via a global port then it will use the port to ensure the connectivity. If you have nets global then you can only get 2 nets on different sheets to connect up if they have the same name (and you will find that if you have 2 nets of the same name and no ports they will still connect up). I have to say that if you use "nets and ports global" then I feel you should be able to work without ports as in a fully annotated cct they change nothing.

from the book with this setting ports only connect to ports of the same name and nets to nets, there is no implicit connection made between ports and nets of the same name

power nets are always global as far as I know (I've never routed them explicitly between sheets and I never had a problem).

I have to say that having switched to using full hierarchical design using a proper project sheet and connecting the relevant parts of the circuit up on that that I have found complex circuits much easier to follow and may fewer ERC problems. I know there are several people out there saying that protel 99sp6 doesn't work well with hierarchical designs but this is exactly contrary to my experience. I admit there was a bit of a learning curve learning to get the project sheet accurate etc. but it is just a case of doing the connecting up what you want connected the same as on the basic sheets.

my standard setting for all projects now are "sheet symbol/port connections", "descend into sheet parts" and "append sheet number to local nets" when creating netlists.

Brad Velander wrote:

        why is the net connectivity called "Net Labels and Ports Global"? This seems 
to be the root of the problem, call it semantics or call it a bug, the statement implies ports 
and nets are both treated globally. But it is becoming apparent that they aren't, the question 
now is? Do the ports perform their connectivity between individual sheets or not, let alone 
        However, in my case I did not even rely on any global connectivity tricks of 
the ports, I wired the desired signals directly to the sheet entries and directly to 
the ports on the subsheet. The ports and sheet entries only had to perform their 
expected connectivity between the master sheet and the subsheet, it failed to do this. 
I still don't know why but according to Craig from Altium, it just plain won't work. 
Possibly he misunderstood my issue and therefore his answer was not correct but he 
seemed pretty sure of the fact that it didn't work because the only way to make ports 
work was by not having any form of nets global in the connectivity setting. Not going 
to happen, I don't need to spend hours connecting multiple sheets together on a top 
level master sheet that nobody will even want to view. Thus I typically use a flat 
hierarchy and global nets. This case was special because they tried to jam too much 
circuitry into a an existing schematic where my only option was to connect through a 
sheetsymbol in place of the former integrated device schematic symbol.

Brad Velander.

Lead PCB Designer
Norsat International Inc.
Microwave Products
Tel   (604) 292-9089 (direct line)
Fax  (604) 292-9010

-----Original Message-----
From: Chris Lowe [mailto:[EMAIL PROTECTED]
Sent: Thursday, July 24, 2003 1:33 AM
To: Protel EDA Forum
Subject: Re: [PEDA] P99SE Sheet Symbol & Port connectivity across

with ports and nets global the Ports have no electrical value, they contribute nothing to the design routing as connectivity is by the globally defined nets. If you wish to connect to local nets with different names via a common named port you must set the net identifier scope to be ports global (or sheet symbol / port connections if you have a project sheet)

chris lowe

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* Contact the list manager:
* Forum Guidelines Rules:
* Browse or Search previous postings:
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to