Re: [PEDA] Power Ports - It can be done!
There used to be a knowledge base item about this but I can't find it now. From memory and experience, however, here's the method of creating custom power objects that behave the same way as the built-in ones: Create your power symbol as a component in a library making sure it satisfies all of the following conditions. 1. It has only one single pin. 2. That pin is hidden. 3. Its type is 'Power'. 4. The name of the pin is the net name you want (e.g.: AGND ) The length of the pin doesn't matter but the point that establishes connectivity to wires and parts is the STEM of the pin NOT the end. You can place these custom power objects as parts in the Schematic Editor. The good news is they won't appear as components in the netlist!!! So the Netlist Manager or the Synchronizer will not try to place footprints for them. To make them 'invisible' even in BOMs use the old trick of making their Part Type field empty. I discovered these special power objects years ago in a schematic design imported from Orcad. Gyula * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Power Ports
Abd ul-Rahman Lomax wrote: > > No, I don't think it would. A power port creates a global net with its name > *and* it connects that net to pins and wires through the hot spot of the > power port. > > A power pin on a component does not create any named net if it is visible; > it will connect, yes, but two of these used, for example, as power sources > for an IC would not connect power to that IC. Hidden pins create nets with > their name, but these nets only connect the pin number of the hidden pin to > the named net; as a hidden pin, it does not establish connectivity to any > other pin. > > *However,* one could make a symbol with no pins with whatever graphic one > wanted and use this, in conjunction with a net name, to create a local > "power" net. The origin of the net name (this is the lower left corner of > the text) should be at the apparent hot spot of this symbol. But I don't > think this would be terribly useful, and it could cause confusion, since we > expect power nets to be global; this object create a local net, i.e., > global only if all nets are global. Thanks much for this clarification. I wasn't sure my idea would work, but you have shown why it would not be a good idea (the local/global difference). Jon * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Power Ports
At 05:25 PM 3/29/2002 -0600, Jon Elson wrote: >I don't think there is >any way to easily add a new symbol to the list, however. I don't know of any way at all. (Except that one can make power ports galore with different power net names, but I don't think that was the question; this is not a new *symbol*.) > On the other hand, >I think you could create a "component", put it in a library, and make up >a menu entry that would select that component with a "Place Part" >command. If the name of the pin in the component is GND or a power >net on your board, and the pin is set as a power pin, it should work just >like any of the predefined power ports. No, I don't think it would. A power port creates a global net with its name *and* it connects that net to pins and wires through the hot spot of the power port. A power pin on a component does not create any named net if it is visible; it will connect, yes, but two of these used, for example, as power sources for an IC would not connect power to that IC. Hidden pins create nets with their name, but these nets only connect the pin number of the hidden pin to the named net; as a hidden pin, it does not establish connectivity to any other pin. *However,* one could make a symbol with no pins with whatever graphic one wanted and use this, in conjunction with a net name, to create a local "power" net. The origin of the net name (this is the lower left corner of the text) should be at the apparent hot spot of this symbol. But I don't think this would be terribly useful, and it could cause confusion, since we expect power nets to be global; this object create a local net, i.e., global only if all nets are global. Yes, we should be able to control the graphics for power ports. We should also have a tool for making the assigned net of a ground power port visible, and ERC should flag any identical symbols which have different nets. This condition is a common error source, where the schematic appears to have a single ground, for example, but there are, in the net list, multiple grounds because the ground ports have been given different names. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Power Ports
Anthony Whitesell wrote: > Does anyone know how (if it is possible) to create a new power port symbol? You're not talking about a menu entry, but the actual picture that goes on the schematic itself? There are 5, I think, different symbols built into Protel that you can set up a custom menu entry for. I don't think there is any way to easily add a new symbol to the list, however. On the other hand, I think you could create a "component", put it in a library, and make up a menu entry that would select that component with a "Place Part" command. If the name of the pin in the component is GND or a power net on your board, and the pin is set as a power pin, it should work just like any of the predefined power ports. I've never had the need to make a new symbol for this purpose, the ones built in have been sufficient. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Power ports
Sean James wrote: > Is there any way to change or create new power port symbols? (I would like > to create a square symbol). Well, it is pretty easy to add a new menu item with an icon of your choice to the MENU that you select these from. BUT, I don't know a way to create an arbitrary symbol and actually have that appear on the SCHEMATIC as a power port, directly. What I think you need to do is create a component which has the graphic representation you like with the schematic library editor, and assign the pin to the power net name you want. This is the rub. A real power port symbol has the net name accessible so you can change it, and it displays right on the schematic. I'm not sure you can do that so easily with the component substitute for that, and you can't pick it from the wiring toolbar. But, if it is important to have the special symbol appearance on the schematic sheet, you can definitely create it as a component. Jon * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Power ports
At 07:59 AM 2/14/2002 -0500, Sean James wrote: >Is there any way to change or create new power port symbols? (I would like >to create a square symbol). The short answer is no, I am afraid. At least I have never heard of one. Protel could give us this facility quite simply, by adding a global power attribute option to the possibilities for pins. Right now, hidden pins will create such a net, but a hidden pin could not serve to connect a visible pin or wire to the net. [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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
