Re: [PEDA] Microstrip footprints
Jami, you need to learn the definition of a bug I guess. Bitch all you want about Protel, I don't care. Just be accurate. You're a professional, not some high school hack. You should be able to refer to a problem as either a bug or a poor implementation, a lack of implementation, or something you just don't like. There is a difference between all four. So here I will be content to simply to state that it is a SUPER GIANT ENORMOUSY GLARING DESIGN OMISSION OF UNPRECIDENTED MAGNITUDE AND PROPORTIONS. YES!!! Tony -Original Message- From: JaMi Smith [mailto:[EMAIL PROTECTED]] Sent: Tuesday, July 23, 2002 3:23 PM To: Protel EDA Forum Cc: JaMi Smith Subject: Re: [PEDA] Microstrip footprints Protel understands nothing of microstrip mitered corners or microstrip components such as inductors. There are two parts to the problem, one concerning unconnected copper, and the other with shorts. The first, unconnected copper, is similar to a question raised here in this forum a while back regarding dual footprints for a crystal, where a library component needs to contain more copper than just a pad or hole, and in that particular instance, a pad and a hole connected together with copper. This is a problem in Protel, and the current Official soultion is to make whatever copper shapes that you need in your library component, and then check the box that says include copper when you are doing an update (syncronizing) from the Schematic to PCB. You can also do a form of this in the Netlist Manager menu, where you can also include the connected copper. This will solve most Netlist problems and DRC errors (except the short, for which see below), but the problem is that you have to remember to do this every time you update, and I hate to use the Netlist Manager functions because they scare me, having on occasion had it short nets together and lose others completely, forcing me to go back to do another update. The real problem is that you should be able to design copper areas within a library component and have those copper areas remain permanently attached, electrically (or netlist) speaking, to whatever electical pad of land it is connected to, but Protel simply isn't smart enough to do that in it's current incarnation. We can only hope it will show up in DXP Service Pack 3 or 4. If I were to call this a bug here in this form, I would instantly be trashed with reasons why it should not be so. So I will be content to state that it is simply a GLARING DESIGN OMISSION. A secondary issue that you will find when you do this is the short. This has been discussed at length here in this forum, and there really is no acceptable way aroud the DRC error problem here (although you can search the archives for the Lomax Short, which some claim to be at least a partial solution to the problem). Here again, the real problem is that you should be able to design copper areas within a library component and have those copper areas remain permanently attached, even if it constitutes a short, but once again Protel simply isn't smart enough to do that in it's current incarnation. Again, calling this a bug here in this form would simply instantly invoke responses. So here I will be content to simply to state that it is a SUPER GIANT ENORMOUSY GLARING DESIGN OMISSION OF UNPRECIDENTED MAGNITUDE AND PROPORTIONS. In answer to your current problem, I would simply design a library component for both PCB and Schematic for your miter, and simply add it to your schematics and also your pcb's and live with the DRC error. I think that you will find that this is what you will have to do with virtually any RF parts such as these miters in transmission lines or certain types of inductors that would constitute a short at DC. Respecting resistors, capacitors and transmission lines, you might find it useful to note that a 20 mil wide pad on an 0402 surface mount R or C mates perfectly with a 20 mil wide 50 ohm line derived with 12 mil of FR4 over a ground plane (assuming you can tolerate FR4 in your design). JaMi Smith [EMAIL PROTECTED] * * * * * * * * * * - Original Message - From: Daniel Webster [EMAIL PROTECTED] To: 'Protel EDA Forum' [EMAIL PROTECTED] Sent: Tuesday, July 23, 2002 10:31 AM Subject: Re: [PEDA] Microstrip footprints Has anyone developed footprints for microstrip sections ? I have been trying to do this with pads set to certain length and widths. Mitered corners are particularly challenging to make as a library footprint. I have used two pads placed side by side at a 45 degree angle with the desired measurements. If I add fills to this footprint to complete the desired pattern then I will get DRC errors on my board once I load a netlist. It would be nice for this situation to have various pad shapes available (user defined), triangular, trapazoidal, etc. If anyone has found a solution, or knows where
Re: [PEDA] Microstrip footprints
Daniel, Ian, there is a further possible design corruption problem when using the Assign Net to Connected Copper function during an update. If you have updated a footprint to a new footprint at the same time that you are updating with the connected copper checked. You can really screw up your database if the new footprint touches some copper that the old part did not, or the new part is in a different rotation and touches some copper (typically GND) that it shouldn't have. The part may be updated, make the illegal connection, then the update copper from connected pads updates the illegally connected copper to the wrong net (usually changing it from GND in my designs). I prefer to run the update, check all existing components in the existing layout (typically only those already placed and routed) to see that they don't make a short to something they shouldn't, then I will run the Netlist Manager, Update Free Primitives From Component Pads function. Sincerely, Brad Velander. Lead PCB Designer Norsat International Inc. Microwave Products Tel (604) 292-9089 (direct line) Fax (604) 292-9010 email: [EMAIL PROTECTED] http://www.norsat.com -Original Message- From: Ian Wilson [mailto:[EMAIL PROTECTED]] Sent: Tuesday, July 23, 2002 4:06 PM To: Protel EDA Forum Subject: Re: [PEDA] Microstrip footprints SNIP When you synchronise from a Sch to the PCB using Tools/Update PCB you can check the Assign Net to Connected Copper check box but I found this made the synch slower than otherwise and by more than the time taken to manually run the Update Free Primitives from Component Pads process - I did not do a careful check though. Ian Wilson * Tracking #: 1AAC93682FBEEE4D8614CDD9E9026534892FEC04 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Microstrip footprints
I did not know about the ability to included unconnected copper. Thanks, that may prove quite useful. As far as the problem of shorts, I have come up with my own solution to this. I place matching netlabels on either ends of the microstrip symbol, so that I maintain a netlist connection. I do not want these netlabels to appear on the schematic when printed so I change their color to white and print in color to the monochrone laser printer. I use a non-white background while working on the netlabels so that they are visible to me, but change the background back to white before printing. This has worked well for me, and removes DRC errors even when the pads used to make the microstrip sections are overlapping each other. My only difficult is with making the odd shapes with fills, etc., and eliminating the DRCs created for the non-pad copper in the footprint. I think if I use the Update Free Primitives from Component Pads command which Ian mentioned, being careful not to create shorts that I do not intend, this will solve my problems temporarily. I appreciate the help on this issue, and hope that Protel will consider adding better utilities for handling microstrip design. Perhaps someone will get ambitious and write a server which creates the microstrip pattern from the information embedded into the schematic symbol. Wouldn't that be slick ! Daniel -Original Message- From: JaMi Smith [mailto:[EMAIL PROTECTED]] Sent: Tuesday, July 23, 2002 3:23 PM To: Protel EDA Forum Cc: JaMi Smith Subject: Re: [PEDA] Microstrip footprints Protel understands nothing of microstrip mitered corners or microstrip components such as inductors. There are two parts to the problem, one concerning unconnected copper, and the other with shorts. The first, unconnected copper, is similar to a question raised here in this forum a while back regarding dual footprints for a crystal, where a library component needs to contain more copper than just a pad or hole, and in that particular instance, a pad and a hole connected together with copper. This is a problem in Protel, and the current Official soultion is to make whatever copper shapes that you need in your library component, and then check the box that says include copper when you are doing an update (syncronizing) from the Schematic to PCB. You can also do a form of this in the Netlist Manager menu, where you can also include the connected copper. This will solve most Netlist problems and DRC errors (except the short, for which see below), but the problem is that you have to remember to do this every time you update, and I hate to use the Netlist Manager functions because they scare me, having on occasion had it short nets together and lose others completely, forcing me to go back to do another update. The real problem is that you should be able to design copper areas within a library component and have those copper areas remain permanently attached, electrically (or netlist) speaking, to whatever electical pad of land it is connected to, but Protel simply isn't smart enough to do that in it's current incarnation. We can only hope it will show up in DXP Service Pack 3 or 4. If I were to call this a bug here in this form, I would instantly be trashed with reasons why it should not be so. So I will be content to state that it is simply a GLARING DESIGN OMISSION. A secondary issue that you will find when you do this is the short. This has been discussed at length here in this forum, and there really is no acceptable way aroud the DRC error problem here (although you can search the archives for the Lomax Short, which some claim to be at least a partial solution to the problem). Here again, the real problem is that you should be able to design copper areas within a library component and have those copper areas remain permanently attached, even if it constitutes a short, but once again Protel simply isn't smart enough to do that in it's current incarnation. Again, calling this a bug here in this form would simply instantly invoke responses. So here I will be content to simply to state that it is a SUPER GIANT ENORMOUSY GLARING DESIGN OMISSION OF UNPRECIDENTED MAGNITUDE AND PROPORTIONS. In answer to your current problem, I would simply design a library component for both PCB and Schematic for your miter, and simply add it to your schematics and also your pcb's and live with the DRC error. I think that you will find that this is what you will have to do with virtually any RF parts such as these miters in transmission lines or certain types of inductors that would constitute a short at DC. Respecting resistors, capacitors and transmission lines, you might find it useful to note that a 20 mil wide pad on an 0402 surface mount R or C mates perfectly with a 20 mil wide 50 ohm line derived with 12 mil of FR4 over a ground plane (assuming you can tolerate FR4 in your design). JaMi Smith [EMAIL PROTECTED] * * * * * * * * * * - Original Message - From: Daniel
Re: [PEDA] Microstrip footprints
Has anyone developed footprints for microstrip sections ? I have been trying to do this with pads set to certain length and widths. Mitered corners are particularly challenging to make as a library footprint. I have used two pads placed side by side at a 45 degree angle with the desired measurements. If I add fills to this footprint to complete the desired pattern then I will get DRC errors on my board once I load a netlist. It would be nice for this situation to have various pad shapes available (user defined), triangular, trapazoidal, etc. If anyone has found a solution, or knows where I can find microstrip footprints, please let me know. Thanks, Daniel * Tracking #: 302C7AEC4E668747A3931191787D4A780F50FC92 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Microstrip footprints
Protel understands nothing of microstrip mitered corners or microstrip components such as inductors. There are two parts to the problem, one concerning unconnected copper, and the other with shorts. The first, unconnected copper, is similar to a question raised here in this forum a while back regarding dual footprints for a crystal, where a library component needs to contain more copper than just a pad or hole, and in that particular instance, a pad and a hole connected together with copper. This is a problem in Protel, and the current Official soultion is to make whatever copper shapes that you need in your library component, and then check the box that says include copper when you are doing an update (syncronizing) from the Schematic to PCB. You can also do a form of this in the Netlist Manager menu, where you can also include the connected copper. This will solve most Netlist problems and DRC errors (except the short, for which see below), but the problem is that you have to remember to do this every time you update, and I hate to use the Netlist Manager functions because they scare me, having on occasion had it short nets together and lose others completely, forcing me to go back to do another update. The real problem is that you should be able to design copper areas within a library component and have those copper areas remain permanently attached, electrically (or netlist) speaking, to whatever electical pad of land it is connected to, but Protel simply isn't smart enough to do that in it's current incarnation. We can only hope it will show up in DXP Service Pack 3 or 4. If I were to call this a bug here in this form, I would instantly be trashed with reasons why it should not be so. So I will be content to state that it is simply a GLARING DESIGN OMISSION. A secondary issue that you will find when you do this is the short. This has been discussed at length here in this forum, and there really is no acceptable way aroud the DRC error problem here (although you can search the archives for the Lomax Short, which some claim to be at least a partial solution to the problem). Here again, the real problem is that you should be able to design copper areas within a library component and have those copper areas remain permanently attached, even if it constitutes a short, but once again Protel simply isn't smart enough to do that in it's current incarnation. Again, calling this a bug here in this form would simply instantly invoke responses. So here I will be content to simply to state that it is a SUPER GIANT ENORMOUSY GLARING DESIGN OMISSION OF UNPRECIDENTED MAGNITUDE AND PROPORTIONS. In answer to your current problem, I would simply design a library component for both PCB and Schematic for your miter, and simply add it to your schematics and also your pcb's and live with the DRC error. I think that you will find that this is what you will have to do with virtually any RF parts such as these miters in transmission lines or certain types of inductors that would constitute a short at DC. Respecting resistors, capacitors and transmission lines, you might find it useful to note that a 20 mil wide pad on an 0402 surface mount R or C mates perfectly with a 20 mil wide 50 ohm line derived with 12 mil of FR4 over a ground plane (assuming you can tolerate FR4 in your design). JaMi Smith [EMAIL PROTECTED] * * * * * * * * * * - Original Message - From: Daniel Webster [EMAIL PROTECTED] To: 'Protel EDA Forum' [EMAIL PROTECTED] Sent: Tuesday, July 23, 2002 10:31 AM Subject: Re: [PEDA] Microstrip footprints Has anyone developed footprints for microstrip sections ? I have been trying to do this with pads set to certain length and widths. Mitered corners are particularly challenging to make as a library footprint. I have used two pads placed side by side at a 45 degree angle with the desired measurements. If I add fills to this footprint to complete the desired pattern then I will get DRC errors on my board once I load a netlist. It would be nice for this situation to have various pad shapes available (user defined), triangular, trapazoidal, etc. If anyone has found a solution, or knows where I can find microstrip footprints, please let me know. Thanks, Daniel * Tracking #: 302C7AEC4E668747A3931191787D4A780F50FC92 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Microstrip footprints
On 10:31 AM 23/07/2002 -0700, Daniel Webster said: Has anyone developed footprints for microstrip sections ? I have been trying to do this with pads set to certain length and widths. Mitered corners are particularly challenging to make as a library footprint. I have used two pads placed side by side at a 45 degree angle with the desired measurements. If I add fills to this footprint to complete the desired pattern then I will get DRC errors on my board once I load a netlist. It would be nice for this situation to have various pad shapes available (user defined), triangular, trapazoidal, etc. If anyone has found a solution, or knows where I can find microstrip footprints, please let me know. Thanks, Daniel Protel does not support complex pads as such. You can achieve what you want with combinations of pads and fills as you are doing. To remove the DRC errors you can use the Update Free Primitives from Component Pads command. This command says free primitives but it will actually update fills and tracks that are part of a footprint. This command is somewhat hidden: Design/Netlist Manager... Click on the Menu button and select Update Free Primitives from Component Pads. When you synchronise from a Sch to the PCB using Tools/Update PCB you can check the Assign Net to Connected Copper check box but I found this made the synch slower than otherwise and by more than the time taken to manually run the Update Free Primitives from Component Pads process - I did not do a careful check though. Ian Wilson * Tracking #: E15F96AD78499A488F1F631A9C6D0D87C69599AD * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *