[PEDA] Schematic Port questions
Two easy ones (I think): (1) I have a multi-page schematic with ports to connect nets between pages. Is there any way, besides adding a net label, to force Protel to give the net the port name in the netlist instead of something like R54_1? Why do I care about net names? Because descriptive names help me when I'm routing. Why don't I want to add a net label? Because then I have a wire with a net label and a port right next to each other -- it just looks silly. (2) I am using the Reports/Add Port References (Flat) feature which works pretty well except that it doesn't seem to generate a reference for ports of the same name on the same page. Is there any way to get the references for ports on the same page? Thanks, Matt __ Do You Yahoo!? LAUNCH - Your Yahoo! Music Experience http://launch.yahoo.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/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Schematic Port questions
At 12:16 PM 5/20/2002 -0700, Embedded Matt wrote: Two easy ones (I think): (1) I have a multi-page schematic with ports to connect nets between pages. Is there any way, besides adding a net label, to force Protel to give the net the port name in the netlist instead of something like R54_1? If you are using a hierarchical schematic, the net will take the name that it has on the highest level on which the net occurs. If the net is not named on that level, it will be given a numerical name. This is not a bug, it is, rather, a necessary consequence of how hierarchical schematics can be used. One may connect WR* on one sheet symbol to CHANNEL1WR* on another sheet symbol. Which name do you give it? Even if the schematic is not flat, suppose one is using Ports Only scope. Using a port, one may connect a net with one name on one sheet to a net with a different name on another sheet. In other words, Net Labels establish a local name (or a global name under certain circumstances, Ports connect between sheets. Ports are not used to name nets. If you are using Net Labels and Ports Global scope, you must place a net label to force the assignment of a net name. With this scope, you don't need to use ports at all But a little redundancy never hurt anyone. Why do I care about net names? Because descriptive names help me when I'm routing. Why don't I want to add a net label? Because then I have a wire with a net label and a port right next to each other -- it just looks silly. Nevertheless, sometimes this is absolutely necessary. (2) I am using the Reports/Add Port References (Flat) feature which works pretty well except that it doesn't seem to generate a reference for ports of the same name on the same page. Is there any way to get the references for ports on the same page? I haven't used that tool, so I'll let someone else answer Except I'll mention that this is not how Ports are designed to be used. They are specifically for intersheet connections. Bring a Port onto a sheet and if you want to use it in various places without having a wire, use multiple net labels. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Schematic Port questions
[snip] Why don't I want to add a net label? Because then I have a wire with a net label and a port right next to each other -- it just looks silly. [snip] Then put the net label on the other end of the wire. In fact, I like to put net labels on both ends of the wire (sometimes in the middle a few times too) on very long wires. And why would I do that you ask? When you are wiring up a schematic with a bunch of parallel wires making 90 degree turns and snaking around components, humans have a tendency to loose the wire they are following. So if you are following a wire and find a net label along the way, you can confirm that you are on the correct wire. Jeff Stout * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Schematic Port questions
On 12:16 PM 20/05/2002 -0700, Embedded Matt said: Two easy ones (I think): (1) I have a multi-page schematic with ports to connect nets between pages. Is there any way, besides adding a net label, to force Protel to give the net the port name in the netlist instead of something like R54_1? No. (2) I am using the Reports/Add Port References (Flat) feature which works pretty well except that it doesn't seem to generate a reference for ports of the same name on the same page. Is there any way to get the references for ports on the same page? There is a 3rd party port annotator available. http://www.aspiring-technology.com/ This third part server has been reported by some to be better than the in-built tool but I have not tested either so can't vouch for that. Ian Wilson * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Schematic Port questions
On 06:28 PM 20/05/2002 -0400, Abd ulRahman Lomax said: At 12:16 PM 5/20/2002 -0700, Embedded Matt wrote: Two easy ones (I think): (1) I have a multi-page schematic with ports to connect nets between pages. Is there any way, besides adding a net label, to force Protel to give the net the port name in the netlist instead of something like R54_1? If you are using a hierarchical schematic, the net will take the name that it has on the highest level on which the net occurs. If the net is not named on that level, it will be given a numerical name. This is not a bug, it is, rather, a necessary consequence of how hierarchical schematics can be used. One may connect WR* on one sheet symbol to CHANNEL1WR* on another sheet symbol. Which name do you give it? Even if the schematic is not flat, suppose one is using Ports Only scope. Using a port, one may connect a net with one name on one sheet to a net with a different name on another sheet. In other words, Net Labels establish a local name (or a global name under certain circumstances, Ports connect between sheets. Ports are not used to name nets. If you are using Net Labels and Ports Global scope, you must place a net label to force the assignment of a net name. With this scope, you don't need to use ports at all But a little redundancy never hurt anyone. Maybe my No answer was less than helpful :-) On a related issue. Do you know that you can use the cloning (or morphing) facility in Protel to quickly grab the text out of a Port while placing net labels? And visa-versa (taking a netlabels text into a port while placing ports). While placing an entity hover over the thing you want to clone and press the INS key. On some objects this can be a little fiddly (getting the right spot) but with a little practice it works well. Morphing can be found in both the on-line help and the printed docs - use the online help Find and enter morph (use the index for the printed stuff). This is a very useful tool in many situations (such as going around adding all your power ports to your design). Ian Wilson * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Schematic Port questions
--- Abd ulRahman Lomax [EMAIL PROTECTED] wrote: If you are using Net Labels and Ports Global scope, you must place a net label to force the assignment of a net name. With this scope, you don't need to use ports at all I don't? Great! But then how do I generate the little strings next to the net labels that tell me what page and grid reference the net goes to? I'll tell you how I've done it in the past -- by hand! It's time consuming and error prone, but necessary. My schematics are typically about 10 pages or so so I need an aid to help me find the other end of the wire. (When I'm debugging in the field, I'm using paper copies.) Ports allow me to automate the process but with two distinct disadvantages over my tedious manual method: 1. It seems impossible to generate references within the same page automatically (without 3rd party tools). 2. The automatically generated references sometimes appear on the wrong side of the port so that the text is placed directly over a wire. Sometimes I can fix this; sometimes I can't. Anybody have any clever ways they handle generating net cross references? I've seen schematics (not drawn in Protel) that include tables at the end with this kind of information. Although, in my opinion, that's not quite as convenient as having the information embedded on every page, if I could generate that kind of table automatically I'd adopt that method in a second. Thanks! Matt __ Do You Yahoo!? LAUNCH - Your Yahoo! Music Experience http://launch.yahoo.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/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Schematic Port questions
At 09:03 AM 5/21/2002 +1000, you wrote: On 12:16 PM 20/05/2002 -0700, Embedded Matt said: Two easy ones (I think): (1) I have a multi-page schematic with ports to connect nets between pages. Is there any way, besides adding a net label, to force Protel to give the net the port name in the netlist instead of something like R54_1? No. (2) I am using the Reports/Add Port References (Flat) feature which works pretty well except that it doesn't seem to generate a reference for ports of the same name on the same page. Is there any way to get the references for ports on the same page? There is a 3rd party port annotator available. http://www.aspiring-technology.com/ This third part server has been reported by some to be better than the in-built tool but I have not tested either so can't vouch for that. Ian Wilson This is a very good tool. A lot better than Protel's attempt. I just hope Protel put's it in their upcoming release. Positioning could be better. Something for Protel to shoot for. Rusty Garfield C. I. D. Development Technician IV Sugar Land Product Center (281) 285-7611 (voice) (281) 285-7619 (fax) [EMAIL PROTECTED] (e-mail) * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
