Re: [PEDA] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name.
Thanks Tony, I am not sure that you are right though. It has persisted across two operating systems/installs on my machine, numerous databases and several other peoples machines at our facility. That is a little more then a chance installation screw-up or corrupted install. If you could please try, in this order, enter a free pad, unplated with no pad diameter, 100 mil hole, Net GND. Then pour a GND polygon over it with pour over same net and remove dead copper. It should flood right over the pad/hole. Now change the Pad netname to No Net and repour. This should be exactly how I have generated this issue repeatedly. Note I think it may have something to do with the unplated hole or 0 size pads. In this case the pad is a tooling hole which I want cleared from the polygon, on the current board this was connected to GND and completely flooded over last build. The other manner in which this could have come about is having the polygon pour first and then placing the free pad into the polygon pour. This would have given it the GND net. Today I changed the net on the pad to No Net and the pour does not clear from the hole. 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 See us at Booth 323 at Satellite 2002 in Washington, DC March 6-8. -Original Message- From: Tony Karavidas [mailto:[EMAIL PROTECTED]] Sent: Tuesday, February 12, 2002 10:03 AM To: Protel EDA Forum Subject: Re: [PEDA] Serious Bug: Polygons still connecting to pads after the net has been changed to something other then the polygon net name. It's your system. I'm not sure exactly what it is, but it works fine here and has worked fine for a long time. I just tried it. If I place a free pad on a poly, it acquires the netname of the poly. If I then change the name to No Net, a pile of DRC green shows up and if I repour the poly, it is now disconnected. Maybe something is crazy with your installation. (which is another topic) -Original Message- From: Brad Velander [mailto:[EMAIL PROTECTED]] Sent: Tuesday, February 12, 2002 9:24 AM To: Protel EDA Forum List Server (E-mail) Subject: [PEDA] Serious Bug: Polygons still connecting to pads after the net has been changed to something other then the polygon net name. P99Se Sp6 on W2K Has anybody else noticed the bug that connects a pad to a polygon after that pad has been changed to a different net? Any solutions, besides deleting the pad and inserting a new one? In our microwave boards we do a lot of polygons with stitched vias and some pads. Time and time again I will change a free pad to a new netname so that it should not connect to the polygon pour. If the pad was previously the same net as the polygon and the polygon had been poured over the pad at least once, changing to the new netname does not isolate the pad from further polygon pours. On future polygon pours of the old polygon, it continues to pour over the pad which is now connected to a different net. It also does not highlight the DRC violation. 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 See us at Booth 323 at Satellite 2002 in Washington, DC March 6-8. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name.
The (design rule) clearance is from the PAD, not the hole -- so a 0-size pad won't leave the clearance you want. The pad needs to match (or nearly) the hole size. -Original Message- From: Brad Velander [mailto:[EMAIL PROTECTED]] Sent: Tuesday, February 12, 2002 10:41 AM snip If you could please try, in this order, enter a free pad, unplated with no pad diameter, 100 mil hole, Net GND. Then pour a GND polygon over it with pour over same net and remove dead copper. It should flood right over the pad/hole. Now change the Pad netname to No Net and repour. This should be exactly how I have generated this issue repeatedly. Note I think it may have something to do with the unplated hole or 0 size pads. In this case the pad is a tooling hole which I want cleared from the polygon, on the current board this was connected to GND and completely flooded over last build. The other manner in which this could have come about is having the polygon pour first and then placing the free pad into the polygon pour. This would have given it the GND net. Today I changed the net on the pad to No Net and the pour does not clear from the hole. Sincerely, Brad Velander. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name.
That works for me too. I did EXACTLY what you said, and as soon as I changed the net to no net, I got DRC on the connection tracks. A repour disconnected the pad. Dunno... -Original Message- From: Brad Velander [mailto:[EMAIL PROTECTED]] Sent: Tuesday, February 12, 2002 10:41 AM To: 'Protel EDA Forum' Subject: Re: [PEDA] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name. Thanks Tony, I am not sure that you are right though. It has persisted across two operating systems/installs on my machine, numerous databases and several other peoples machines at our facility. That is a little more then a chance installation screw-up or corrupted install. If you could please try, in this order, enter a free pad, unplated with no pad diameter, 100 mil hole, Net GND. Then pour a GND polygon over it with pour over same net and remove dead copper. It should flood right over the pad/hole. Now change the Pad netname to No Net and repour. This should be exactly how I have generated this issue repeatedly. Note I think it may have something to do with the unplated hole or 0 size pads. In this case the pad is a tooling hole which I want cleared from the polygon, on the current board this was connected to GND and completely flooded over last build. The other manner in which this could have come about is having the polygon pour first and then placing the free pad into the polygon pour. This would have given it the GND net. Today I changed the net on the pad to No Net and the pour does not clear from the hole. 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 See us at Booth 323 at Satellite 2002 in Washington, DC March 6-8. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name.
Thanks Dwight, that does make some sense. Seems I couldn't see the forest for the trees this morning. 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 See us at Booth 323 at Satellite 2002 in Washington, DC March 6-8. -Original Message- From: Dwight [mailto:[EMAIL PROTECTED]] Sent: Tuesday, February 12, 2002 11:01 AM To: 'Protel EDA Forum' Subject: Re: [PEDA] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name. The (design rule) clearance is from the PAD, not the hole -- so a 0-size pad won't leave the clearance you want. The pad needs to match (or nearly) the hole size. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name.
Wayne, that is one variation of a similar problem that I can confirm as well. I haven't had it in the couple of weeks but will probably experience it soon again. Yes, I have verified this problem repeatedly but couldn't find the solution (short of deletion and starting over) or the particulars which might isolate it. As a matter of fact I believe that that problem was coercing/blinding me a little to the issue of pad/hole for DRC spacing which I ran into this morning. Clouded my thoughts while remembering your little problem from weeks past. 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 See us at Booth 323 at Satellite 2002 in Washington, DC March 6-8. -Original Message- From: Wayne Trow [mailto:[EMAIL PROTECTED]] Sent: Tuesday, February 12, 2002 11:39 AM To: Protel EDA Forum Subject: Re: [PEDA] Serious Bug: Polygons still connecting to pads after the net has been changed to something other then the polygon net name. Brad, Ive had this problem with keepout tracks. I place the track to control where the polygon will pour therefore the polygon is there when I place the track hence the track picks up the net name. I edit the porperties of the track and change from GND (usually) to No_Net and check keepout. The online drc then shows the error as it should. BUT If I repour the polygon it ignores the different net keepout and acts as if the keepout isn't even there. Similar but different problem. Thanks Wayne Trow PCB Design Technician Gallagher Group LTD Hamilton NEW ZEALAND [p] +64 7 838 9800 ext 8737 [f] +64 7 838 9801 [e] [EMAIL PROTECTED] |-+ | | Brad Velander | | | BVelander@norsat| | | .com| | || | | 13/02/2002 06:23 | | | Please respond to| | | Protel EDA | | | Forum | | || |-+ --- ---| | | | To: Protel EDA Forum List Server (E-mail) [EMAIL PROTECTED] | | cc: | | Subject: [PEDA] Serious Bug: Polygons still connecting to pads after the net has been changed to | |something other then the polygon net name. | --- ---| P99Se Sp6 on W2K Has anybody else noticed the bug that connects a pad to a polygon after that pad has been changed to a different net? Any solutions, besides deleting the pad and inserting a new one? In our microwave boards we do a lot of polygons with stitched vias and some pads. Time and time again I will change a free pad to a new netname so that it should not connect to the polygon pour. If the pad was previously the same net as the polygon and the polygon had been poured over the pad at least once, changing to the new netname does not isolate the pad from further polygon pours. On future polygon pours of the old polygon, it continues to pour over the pad which is now connected to a different net. It also does not highlight the DRC violation. 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 See us at Booth 323 at Satellite 2002 in Washington, DC March 6-8. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name.
Just had this happen to me (see below). I moved the keepout tracks away from the polygon, repoured the polygon, moved the keepout tracks back into position, repoured again, this time keepouts are recognized?! Duane Foster -Original Message- From: Wayne Trow [mailto:[EMAIL PROTECTED]] Sent: Tuesday, February 12, 2002 11:39 AM To: Protel EDA Forum Subject: Re: [PEDA] Serious Bug: Polygons still connecting to pads after the net has been changed to something other then the polygon net name. Brad, Ive had this problem with keepout tracks. I place the track to control where the polygon will pour therefore the polygon is there when I place the track hence the track picks up the net name. I edit the porperties of the track and change from GND (usually) to No_Net and check keepout. The online drc then shows the error as it should. BUT If I repour the polygon it ignores the different net keepout and acts as if the keepout isn't even there. Similar but different problem. Thanks Wayne Trow PCB Design Technician * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name.
I am sure that Dwight got the right answer for me. The issue is the 0mil pads size. My mind was clouded by the other recent issue as Wayne mentioned with the layer specific keepouts. It was clouding my thoughts about this particular problem I saw this morning. I assume that you used a pad of some 0mil size when you did your test. 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 See us at Booth 323 at Satellite 2002 in Washington, DC March 6-8. -Original Message- From: Tony Karavidas [mailto:[EMAIL PROTECTED]] Sent: Tuesday, February 12, 2002 11:56 AM To: Protel EDA Forum Subject: Re: [PEDA] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name. That works for me too. I did EXACTLY what you said, and as soon as I changed the net to no net, I got DRC on the connection tracks. A repour disconnected the pad. Dunno... * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name.
Agreed... What you want is a 100mil pad with a 100mil hole, and the plated option unchecked. In fact, you shouldn't even need to specify any net if this is just a hole in the board. -- Mike Pilawa - Critical Link, LLC E-Mail: [EMAIL PROTECTED] Voice: 315.425.4045 x206 Fax: 315.425.4048 Address: 251 Salina Meadows Pkwy. Syracuse, NY 13212 WEB: http://www.criticallink.com Dwight wrote: The (design rule) clearance is from the PAD, not the hole -- so a 0-size pad won't leave the clearance you want. The pad needs to match (or nearly) the hole size. -Original Message- From: Brad Velander [mailto:[EMAIL PROTECTED]] Sent: Tuesday, February 12, 2002 10:41 AM snip If you could please try, in this order, enter a free pad, unplated with no pad diameter, 100 mil hole, Net GND. Then pour a GND polygon over it with pour over same net and remove dead copper. It should flood right over the pad/hole. Now change the Pad netname to No Net and repour. This should be exactly how I have generated this issue repeatedly. Note I think it may have something to do with the unplated hole or 0 size pads. In this case the pad is a tooling hole which I want cleared from the polygon, on the current board this was connected to GND and completely flooded over last build. The other manner in which this could have come about is having the polygon pour first and then placing the free pad into the polygon pour. This would have given it the GND net. Today I changed the net on the pad to No Net and the pour does not clear from the hole. Sincerely, Brad Velander. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name.
I spoke a bit too soon -- on my PCB it looks like pads vias are treated differently. Vias use the pad size, and so exhibit the problem. For free pads, the pour leaves an area the shape of the pad (round, rectangular, or octagonal), but uses the larger of the hole and pad size in each direction. (Try a skinny rectangular pad, e.g., 1x50 with a 20mil hole.) -Original Message- From: Brad Velander [mailto:[EMAIL PROTECTED]] Sent: Tuesday, February 12, 2002 11:58 AM Thanks Dwight, that does make some sense. Seems I couldn't see the forest for the trees this morning. Sincerely, Brad Velander. -Original Message- From: Dwight [mailto:[EMAIL PROTECTED]] Sent: Tuesday, February 12, 2002 11:01 AM The (design rule) clearance is from the PAD, not the hole -- so a 0-size pad won't leave the clearance you want. The pad needs to match (or nearly) the hole size. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name.
Tony, I have to reneg on the fact that the problem is related only to the pad size. I am running in circles this morning and just now had a chance to get back in the database and check Dwight's solution. It is not related to pad size. For those who just have to know the outcome! Read on. The problem was related to DRC rules. I had a rule specified to clear the polygon around the tooling holes. This rule does obviously work with the hole size because all of my tooling hole pads are 0 mils. The one hole did not meet the rule requirement (it was at first net GND) because I had specified the rule having NO Net on the tooling holes. This is why the GND flood poured over initially. After changing the net back to NO Net the rule should have worked and did not until I copied one of the other two pads to replace the violating pad. After having connected as the pad being net GND, the pad, DRC or the polygon was obviously corrupted and would not properly clear the pad when it was renamed to No Net. The rule obviously does clear from the hole rather then the pad because it normally works just fine as long I name the tooling hole net as No Net ( and it was not previously connected to GND). The rule is set as follows: ItemA: Bottom Layer, Polygon, Net - Gnd ItemB: Pad Specification 63.5mils, No Net, Multilayer, TOPMidBot X-0 Y-0 Shape-Round. Different nets, 10 mils. This rule will clear 10 mil from the pad hole size rather then the pad size. I believe that the problem mentioned with keepouts may be very similarly related to rules definitions because in the previous experience I had, which was similar to Wayne's comments, I was also using a rule to clear the polygon from the layer specific keepouts. After the one segment of line had been netted to GND, the flood continued to pour right over the keepout even after I had changed the net on the one segment back to no net. So I still think this is a bug! Can anybody confirm it now that I believe I have sorted out all the details surrounding it. Any body wants to see my database, I can cleanse it IP wise and share it later today (after I get my files all panelized and out for quotation. 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 See us at Booth 323 at Satellite 2002 in Washington, DC March 6-8. -Original Message- From: Tony Karavidas [mailto:[EMAIL PROTECTED]] Sent: Tuesday, February 12, 2002 11:56 AM To: Protel EDA Forum Subject: Re: [PEDA] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name. That works for me too. I did EXACTLY what you said, and as soon as I changed the net to no net, I got DRC on the connection tracks. A repour disconnected the pad. Dunno... -Original Message- From: Brad Velander [mailto:[EMAIL PROTECTED]] Sent: Tuesday, February 12, 2002 10:41 AM To: 'Protel EDA Forum' Subject: Re: [PEDA] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name. Thanks Tony, I am not sure that you are right though. It has persisted across two operating systems/installs on my machine, numerous databases and several other peoples machines at our facility. That is a little more then a chance installation screw-up or corrupted install. If you could please try, in this order, enter a free pad, unplated with no pad diameter, 100 mil hole, Net GND. Then pour a GND polygon over it with pour over same net and remove dead copper. It should flood right over the pad/hole. Now change the Pad netname to No Net and repour. This should be exactly how I have generated this issue repeatedly. Note I think it may have something to do with the unplated hole or 0 size pads. In this case the pad is a tooling hole which I want cleared from the polygon, on the current board this was connected to GND and completely flooded over last build. The other manner in which this could have come about is having the polygon pour first and then placing the free pad into the polygon pour. This would have given it the GND net. Today I changed the net on the pad to No Net and the pour does not clear from the hole. 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 See us at Booth 323 at Satellite 2002 in Washington, DC March 6-8. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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: *
Re: [PEDA] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name.
Nope. It WAS zero mils as instructed. Pretty strange huh? (The fact that we all don't get the same outcome) Tony -Original Message- From: Brad Velander [mailto:[EMAIL PROTECTED]] Sent: Tuesday, February 12, 2002 12:14 PM To: 'Protel EDA Forum' Subject: Re: [PEDA] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name. I am sure that Dwight got the right answer for me. The issue is the 0mil pads size. My mind was clouded by the other recent issue as Wayne mentioned with the layer specific keepouts. It was clouding my thoughts about this particular problem I saw this morning. I assume that you used a pad of some 0mil size when you did your test. 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 See us at Booth 323 at Satellite 2002 in Washington, DC March 6-8. -Original Message- From: Tony Karavidas [mailto:[EMAIL PROTECTED]] Sent: Tuesday, February 12, 2002 11:56 AM To: Protel EDA Forum Subject: Re: [PEDA] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name. That works for me too. I did EXACTLY what you said, and as soon as I changed the net to no net, I got DRC on the connection tracks. A repour disconnected the pad. Dunno... * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name.
Yeah, I think I nailed it down Dwight. See my message posted right after this one from you. 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 See us at Booth 323 at Satellite 2002 in Washington, DC March 6-8. -Original Message- From: Dwight [mailto:[EMAIL PROTECTED]] Sent: Tuesday, February 12, 2002 12:37 PM To: 'Protel EDA Forum' Subject: Re: [PEDA] Serious Bug: Polygons still connecting to pads after t he net has been changed to something other then the polygon net name. I spoke a bit too soon -- on my PCB it looks like pads vias are treated differently. Vias use the pad size, and so exhibit the problem. For free pads, the pour leaves an area the shape of the pad (round, rectangular, or octagonal), but uses the larger of the hole and pad size in each direction. (Try a skinny rectangular pad, e.g., 1x50 with a 20mil hole.) * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
