At 11:31 AM 1/31/2002 -0500, Jeff Adolphs wrote: >I didn't know what you did was possible. I use net labels on each pin >such as A0, A1, A2,... I was using comment text to label the buss line >such as AD<7:0>. > >The net label on each pin really gets the signal to the right place. I >always use Global nets because I always have multiple sheets and need >the nets to connect to other pages.
First of all, net labels make actual connections within a sheet. This is not changeable. What is optional is how off-sheet connectivity is handled. Mr. Adolphs uses Net Labels and Ports global. In this case, Ports and Net Labels are equivalent. This is not true with the other connectivity scopes. With Port and Net Labels global, bus labels have no function. But I would recommend using them anyway, instead of text, because someday one might want to use the other scopes. > I also use a graphic oval as an >offpage symbol so the net label is what makes the connection. Like the use of annotation text for net bus labels, this is not only unnecessary, it is fraught with risk. Ports are designed for off-sheet connections. I highly recommend using -- at least -- Only Ports Global connectivity, it forces one to make off-sheet connections visible. I actually recommend going beyond that to Sheet Symbol/Port connections, but it does require more work. That work returns better intersheet checking and clearer documentation. Here is how they work. Only Ports Global causes Net Labels to only create connectivity for the sheet on which they occur. Presumably one allows the netlister to add sheet numbers to the nets when using this scope, otherwise one will get duplicated net names, which I think doesn't work for PCB, I forget. Ports, however, create global nets which connect across sheets to Ports on other sheets with the same name. If you set the port electrical characteristics correctly, this will also allow you to check a single sheet for electrical rules compliance. Electrical rules compliance is not just a detail. A high percentage of schematic errors will show up as a violation of electrical rules, or they will at least produce a warning if you have the Rules matrix properly configured. I recommend creating a warning for all unconnected pins, and then suppressing the warnings with No-ERC directives placed on the pins; the markers serve as a visible notation that one is deliberating leaving a pin open. If the pin has a net name on it, you might assume that it is connected elsewhere, which will not be true if there is some even slight variation in Net Label name, such as AD0 and ADO. Now, Sheet Symbol/Port connectivity is even more clear. It works with hierarchical schematics, and any multi-sheet schematic can be set up as a hierarchical schematic. One has a project page with sheet symbols on it for all the other pages. The same thing is done with the other scopes with flat schematics, to tie the sheets together for netlisting and other purposes, but with this connectivity, nets are only connected between sheets by explicit wires or net labels on a higher-level sheet. So the project page might only consist of sheet symbols and connections between them, or it might have its own circuitry and then all links between it and subsheets are made through the Sheet Symbols. So from one sheet -- in many cases -- you can see all the connectivity for the whole project, excepting only intrasheet connectivity on subsheets. This can be used to make a highly understandable schematic, something which can otherwise become difficult where there are multiple sheets. The advantages of SS/P connectivity become really high with design re-use. One does not need to worry about the details of net naming on the subsheets. Subsheet Net labels are irrelevant for intersheet connectivity, only the explicit connections made at the level above matter. You can have a port named /WR on the subsheet, which will connect to a sheet entry of the same name on this sheet's sheet symbol. This then could be wired to a net named RD on the higher-level sheet. This connectivity can be a bit tricky to get working, it must be done exactly right. But the good news is that if you don't get it right, you will get warnings and errors unless you have misconfigured the ERC matrix. I do not recommend using different names for nets as I mentioned was possible, it is only that with design re-use, one can accept such differences. A proven subsheet does not need to be edited to make it usable, except for adding or changing Ports if necessary. If it is not difficult, by all means, make those Ports have the same names as the Net Labels. But you don't have to, except with Buses. Now, to buses with SS/P connectivity. This works: Subsheet has bus D[0..7] which connects to Net Labels AD0 through AD7. This bus is connected to a Port named D[0..7] Supersheet has a Sheet Symbol referring to the subsheet. That sheet symbol contains a Sheet Entry named the same as the Port on the subsheet, in this case AD[0..7]. That Entry is connected to a Bus Label (Net Label}, presumably with the same name (but this is not necessary -- it appears that the nets are assigned based on sequence, not on name. Here is where AD[0..7] *might* be different from AD[7..0]). The Bus Label connects to its subnet Net Labels on the supersheet. There is a question about the electical characteristics of Ports and Sheet Entries. In my view, these stand in for, i.e., represent, what is off-sheet. So an output on one sheet will be connected to an input Port on the same sheet. Connecting it to an output port, the way I have my error matrix configured, I forget if this is the default, will generate a warning. But this input Port is made to look physically like an Output, ie., I'd prefer to have it on the right-hand side of the schematic if this is easy, and I will definitely make it right-pointing if I can. This port then connects to a Sheet Entry on the sheet's Symbol on the next level. That Entry will have an Output characteristic, so it will correctly drive inputs. It represents what is off-sheet. [EMAIL PROTECTED] Abdulrahman Lomax Easthampton, Massachusetts USA * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
