Re: [PEDA] SV: SV: Unplated SMD-pads??
You could find one pad of a component that is at fault, open the library file and change the relevant properties of one pad of that device and then use the "global" change command. You can specify what properties to match and change in this screen. All SMD pads should be plated, because Protel doesn't like it if not!! Once you have updated all the pads of the component, by one simple process, save the changes to the library, and then click the "update PCB" button. This will update all the pads for any of those components on your PCB, providing the PCB file is open when you click the update button. You can then do this for any offending components. Steve -Original Message- From: Tommy Åkesson [mailto:[EMAIL PROTECTED]] Sent: 13 August 2001 19:19 To: Protel EDA Forum Subject: [PEDA] SV: SV: Unplated SMD-pads?? No cant find any. But if its a multilayer but not plated?. How can i find this?? Okej I know the hard way, click on every pad and check propertys. This will take hours. Tommy -Ursprungligt meddelande- Från: Bob Fearon [mailto:[EMAIL PROTECTED]] Skickat: den 13 augusti 2001 18:02 Till: Protel EDA Forum Ämne: Re: [PEDA] SV: Unplated SMD-pads?? They should show up on the screen as a different color ( multilayer color) instead of top layer or bottom layer. Tommy kesson wrote: > Okej, perhaps... But how do I find them? > > Tommy > > -Ursprungligt meddelande- > Fr n: Bob Fearon [mailto:[EMAIL PROTECTED]] > Skickat: den 13 augusti 2001 15:55 > Till: Protel EDA Forum > mne: Re: [PEDA] Unplated SMD-pads?? > > Tommy > Do you have any of your SMD pads set as multilayer? > I have only seen this message when I made that mistake. > Bob > > Tommy kesson wrote: > > > Sometime then I do DRC I get an error message. > > "Broken-nets contraint" > > Net GND > > Warning nets constain unpladet pads. > > > > How do I find this unplated pads!!! > > Wy must SMD-pads bee plated!!! > > > > Any comments or suggestions?? > > > > Regards > > Tommy * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] SV: SV: Unplated SMD-pads??
Been there, done that, had the error flagged by PCB manufacturer and spent many a happy hour trying to locate the non-plated pad. I located it by exporting all the pads to Spread sheet and scanning down the "plated" column. Note the XY co-ordinates and jump to location on PCB. In my case it was one or two pads on one of my library footprints was in error. The other way (as explained by people who use Protel PCB as a living) is use global select to select all pads with 0mil hole and not plated and then jump to selection. It appears, as they knew the solution instantly, that this non-plated pad "error" occurs quite often. Ian Middleton > -Original Message- > From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED]] > Sent: 13 August 2001 22:22 > To: Protel EDA Forum > Cc: [EMAIL PROTECTED]; [EMAIL PROTECTED] > Subject: Re: [PEDA] SV: SV: Unplated SMD-pads?? > > > I've seen this happen with both Multilayer and top only > SMD...just happened > to me yesterday... > > Best way to find it is to look at the report (menu - Reports - Board > Information - then generate the report by setting to all). You'll see a > heading for non-plated hole sizes like so: > > > Non-Plated Hole Size PadsVias > > 0mil (0mm) 4 0 > 26mil (0.6604mm) 2 0 > 28mil (0.7112mm) 1 0 > 42mil (1.0668mm) 1 0 > 80mil (2.032mm) 2 0 > 94mil (2.3876mm) 5 0 > 96mil (2.4384mm) 6 0 > 104mil (2.6416mm)2 0 > 110mil (2.794mm) 8 0 > 124mil (3.1496mm)3 0 > 125mil (3.175mm) 1 0 > 128mil (3.2512mm)2 0 > 157mil (3.9878mm)2 0 > > Total 39 0 > > > Yours will have different data of course. > > It happened to me with a PADS generated footprint (yea the 901 > pin BGA I've > posted about before) that I grabbed from a PADS ASCII import. > > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] SV: SV: Unplated SMD-pads??
I've seen this happen with both Multilayer and top only SMD...just happened to me yesterday... Best way to find it is to look at the report (menu - Reports - Board Information - then generate the report by setting to all). You'll see a heading for non-plated hole sizes like so: Non-Plated Hole Size PadsVias 0mil (0mm) 4 0 26mil (0.6604mm) 2 0 28mil (0.7112mm) 1 0 42mil (1.0668mm) 1 0 80mil (2.032mm) 2 0 94mil (2.3876mm) 5 0 96mil (2.4384mm) 6 0 104mil (2.6416mm)2 0 110mil (2.794mm) 8 0 124mil (3.1496mm)3 0 125mil (3.175mm) 1 0 128mil (3.2512mm)2 0 157mil (3.9878mm)2 0 Total 39 0 Yours will have different data of course. It happened to me with a PADS generated footprint (yea the 901 pin BGA I've posted about before) that I grabbed from a PADS ASCII import. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
