Re: [PEDA] Place Port vs. place offpage connectors
On 09:40 AM 14/11/2003, Protel Hell said: thank you Ian, I have seen people use alpha/numerics or just numbers or letters to name ports (ports called something else in other schematic capture programs) and some use net names. Is there a naming scheme that works best in Protel? Some of the schematics I've inherited have net names different than port name, which in some cases seems confusing. Protel will support this sort of thing - that is nets having different names from ports. In the past pretty much only netlabels and power objects named nets, ports and sheet entries did not. In DXP ports and sheet entries can name nets but there are some gotchas there (a port labelled net is not the same as a net-labelled net - there is detailed discussion of this elsewhere). In full hierarchical design ports connect to sheet entries on the next higher sheet, sheet entries connect to other sheet entries via wires or busses. There can be many different names for the same net. DXP has a good navigator that helps figure all this out (after you "compile" the design). The simplest scheme, where you can do this, is to simply use the same port and net labels for the same net throughout the design. Oh...and add a net label to every net that has a port, you only need to add the netlabel once somewhere but I usually add a net label next to the port at every port instance. In other design scenarios, where this is not possible, you need to take some care to check you understand the interconnection (use the Navigator, or create and print a netlist and go through it with a highlighter). You should only need to do this a couple of time until you are confident of the results. DXP will give warnings of nets having multiple names when it detects this. hope nobody is offended by my name, I hope to be in Protel Heaven soon. Need to know 3 different CAD here, so it's a little like hell right now. This list is often getting questions about comprehensive, detailed, rational and fair comparisons between CAD packages - have you any comments? What about in 6 months time when you have decent experience all round? I would be very interested in such a post or even article. If you wanted to post on the Altium DXP forum you may want to give yourself a different moniker though. Ian * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Place Port vs. place offpage connectors
On 08:16 AM 14/11/2003, Ian Wilson said: On 01:06 AM 14/11/2003, Protel Hell said: Hi all, Protel DXP newbie here, many years using other CAD tools (PADS, Orcad mainly), with basic question: what is the difference between ports & offpage connectors, when is each used and why? what advantage does one have over the other? Ports are the normal sort means of connecting signals from one sheet to another in Protel products (assuming you are not using a Ports Global naming scheme). Off sheet connectors are provided mainly to provide support for Orcad imports, I understand. They are new in DXP. Unless you expect to be going back and forth to Orcad you can probably stay with ports. Many DXP designs will use only ports. Off sheet connectors are more rarely used. There has been quite a bit of discussion of the off sheet connector and when and how to use it on the DXP forum. I just tried searching the archive but couldn't find the stuff I am sure is there. There seem to be some problems with searching the archive. Some more info. The DXP forum can't seem to search back far enough to find these replies so I dug them out of my own email archive. The following quote is from an Altium employee. I won't mention names but since it is available, at least theoretically, on the public DXP forum I don't think there should be a problem quoting here: Say you created a hierarchical design, meaning that your regular ports don't connect sheets in a flat way, but vertically up to sheet entries on their parent sheets. Then suppose that one of your sheets grew too big, and you wanted to divide it into two or more sheets, but you wanted them to be treated like one sheet. This is what off-sheet connectors can do: they can create a subsection of flat connectivity within a greater hierarchical design. Read the Net Connectivity and Navigation article, esp. the part on Grouped Sheets. Notice that you group sheets by pointing the sheet symbol at multiple sheets, separated by semicolons. Our primary motivation for adding Off-Sheet Connectors was to facilitate imports of OrCAD designs into nVisage. Later the further qualification was added: Benefits of off-sheet connectors over ports? You usually don't have a choice to use one over the other. But I guess if I had a hierarchical schematic set up, and I wanted to plug in a multi-page subcircuit that was designed using flat (ports global) connectivity, I'd like the fact that I didn't have to restructure the subcircuit design to fit into the hierarchy. Instead, I could just replace its ports with off-sheet connectors, then place a single sheet symbol in the greater hierarchy that references all of the sheets in the subcircuit design. (By the way, that's what a sub-divided sheet symbol is referring to: single sheet symbol, multiple sheet names). I guess the way to think of off-sheet connectors is that they give you a limited scope of flat connectivity in a vertical world. But really, we didn't add this new feature to radically revise the way users design their projects. It was primarily a means of maintaining connectivity in the schematics imported from OrCAD. I have not read the Net Connectivity and Navigation article, so I don't know if it makes much mention of off-sheet connectors. Ian * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Place Port vs. place offpage connectors
thank you Ian, I have seen people use alpha/numerics or just numbers or letters to name ports (ports called something else in other schematic capture programs) and some use net names. Is there a naming scheme that works best in Protel? Some of the schematics I've inherited have net names different than port name, which in some cases seems confusing. hope nobody is offended by my name, I hope to be in Protel Heaven soon. Need to know 3 different CAD here, so it's a little like hell right now. From: Ian Wilson <[EMAIL PROTECTED]> Reply-To: "Protel EDA Forum" <[EMAIL PROTECTED]> To: "Protel EDA Forum" <[EMAIL PROTECTED]> Subject: Re: [PEDA] Place Port vs. place offpage connectors Date: Fri, 14 Nov 2003 08:16:02 +1100 On 01:06 AM 14/11/2003, Protel Hell said: Hi all, Protel DXP newbie here, many years using other CAD tools (PADS, Orcad mainly), with basic question: what is the difference between ports & offpage connectors, when is each used and why? what advantage does one have over the other? Ports are the normal sort means of connecting signals from one sheet to another in Protel products (assuming you are not using a Ports Global naming scheme). Off sheet connectors are provided mainly to provide support for Orcad imports, I understand. They are new in DXP. Unless you expect to be going back and forth to Orcad you can probably stay with ports. Many DXP designs will use only ports. Off sheet connectors are more rarely used. There has been quite a bit of discussion of the off sheet connector and when and how to use it on the DXP forum. I just tried searching the archive but couldn't find the stuff I am sure is there. There seem to be some problems with searching the archive. DXP has a number of scopes for nets and ports. By default DXP willl attempt to figure out what sort of scope it should use based on your use of sheet entries and ports. You can override the automatic selection of scope in the Project Options dialog. Click in the drop list and hit F1 for help. Ian _ MSN Shopping upgraded for the holidays! Snappier product search... http://shopping.msn.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Place Port vs. place offpage connectors
On 01:06 AM 14/11/2003, Protel Hell said: Hi all, Protel DXP newbie here, many years using other CAD tools (PADS, Orcad mainly), with basic question: what is the difference between ports & offpage connectors, when is each used and why? what advantage does one have over the other? Ports are the normal sort means of connecting signals from one sheet to another in Protel products (assuming you are not using a Ports Global naming scheme). Off sheet connectors are provided mainly to provide support for Orcad imports, I understand. They are new in DXP. Unless you expect to be going back and forth to Orcad you can probably stay with ports. Many DXP designs will use only ports. Off sheet connectors are more rarely used. There has been quite a bit of discussion of the off sheet connector and when and how to use it on the DXP forum. I just tried searching the archive but couldn't find the stuff I am sure is there. There seem to be some problems with searching the archive. DXP has a number of scopes for nets and ports. By default DXP willl attempt to figure out what sort of scope it should use based on your use of sheet entries and ports. You can override the automatic selection of scope in the Project Options dialog. Click in the drop list and hit F1 for help. Ian * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
[PEDA] Place Port vs. place offpage connectors
Hi all, Protel DXP newbie here, many years using other CAD tools (PADS, Orcad mainly), with basic question: what is the difference between ports & offpage connectors, when is each used and why? what advantage does one have over the other? thank you in advance _ Concerned that messages may bounce because your Hotmail account is over limit? Get Hotmail Extra Storage! http://join.msn.com/?PAGE=features/es * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
