Re: [PEDA] How to place non-plated thru holes?
Actually, I misspoke. I was thinking of a negative annular ring. I actually make my pads 10 mils smaller than the hole size. This just makes it easier to set up plane clearance and solder mask rules. Regards, Steve Smith, C.I.D. Product Engineer Staco Energy Products Co. Web Site: www.stacoenergy.com www.stacopower.com -Original Message- From: Dennis Saputelli [mailto:[EMAIL PROTECTED] Sent: Thursday, October 30, 2003 5:16 PM To: Protel EDA Forum Subject: Re: [PEDA] How to place non-plated thru holes? i don't think 5mils smaller is smaller enough i bet the fabricator tweaks them down it would be nice to get a definitive answer about this we usually make NPTs about 10mil pad size sometimes differents sizes by a few mils for different hole sizes just to make sorting them out easier Dennis Saputelli Steve Smith wrote: Stuart, Place a Pad where you want the hole. I make the pad about 5 mils smaller that the hole size I want. Double click on the pad the go to the Advanced tab and uncheck Plated. Under Properties you can select your pad hole size. In the design rules under Power Plane Clearance set a rule for that pad size that will give you the plane clearance that you want. Regards, Steve Smith, C.I.D. Product Engineer Staco Energy Products Co. Web Site: www.stacoenergy.com www.stacopower.com -Original Message- From: Website Visitor [mailto:[EMAIL PROTECTED] Sent: Thursday, October 30, 2003 5:06 AM To: proteledaforum Subject: [PEDA] How to place non-plated thru holes? Hello -- I was directed to this group as the place where most Protel experts hung out. I am a newbie to Protel and am using Protel99 SE for PCB layout. My question is simple: I want to place a non-plated through hole on my design. I want to void out the plane layers around the hole also. How do I do it? It appears that I can either place a pad or a via, but neither is really a through hole, and it's not obvious (to me, at least) that they will correctly void out the plane layer. Thanks in advance for your wisdom, Stuart Posted from Association web site by: Stuart Brorson -- Dennis Saputelli = send only plain text please! - no HTML == ___ Integrated Controls, Inc. www.integratedcontrolsinc.com 2851 21st Streettel: 415-647-0480 San Francisco, CA 94110 fax: 415-647-3003 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
[PEDA] How to place non-plated thru holes?
Hello -- I was directed to this group as the place where most Protel experts hung out. I am a newbie to Protel and am using Protel99 SE for PCB layout. My question is simple: I want to place a non-plated through hole on my design. I want to void out the plane layers around the hole also. How do I do it? It appears that I can either place a pad or a via, but neither is really a through hole, and it's not obvious (to me, at least) that they will correctly void out the plane layer. Thanks in advance for your wisdom, Stuart Posted from Association web site by: Stuart Brorson * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] How to place non-plated thru holes?
Stuart, Place a Pad where you want the hole. I make the pad about 5 mils smaller that the hole size I want. Double click on the pad the go to the Advanced tab and uncheck Plated. Under Properties you can select your pad hole size. In the design rules under Power Plane Clearance set a rule for that pad size that will give you the plane clearance that you want. Regards, Steve Smith, C.I.D. Product Engineer Staco Energy Products Co. Web Site: www.stacoenergy.com www.stacopower.com -Original Message- From: Website Visitor [mailto:[EMAIL PROTECTED] Sent: Thursday, October 30, 2003 5:06 AM To: proteledaforum Subject: [PEDA] How to place non-plated thru holes? Hello -- I was directed to this group as the place where most Protel experts hung out. I am a newbie to Protel and am using Protel99 SE for PCB layout. My question is simple: I want to place a non-plated through hole on my design. I want to void out the plane layers around the hole also. How do I do it? It appears that I can either place a pad or a via, but neither is really a through hole, and it's not obvious (to me, at least) that they will correctly void out the plane layer. Thanks in advance for your wisdom, Stuart Posted from Association web site by: Stuart Brorson * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] How to place non-plated thru holes?
Place a multilayer thru-hole pad with the hole size you want. Edit the pad such that the pad is smaller than the hole, and uncheck the plated box on the advanced tab. Making the pad smaller than the hole causes the drilling operation to wipe out all copper from the hole on internal signal layers. The plane clearance is based on the hole size, and is determined by the design rules you set for the board, region, component, etc. under the menu DesignRulesManufacturingPower Plane Clearance. Include notes on your drill drawing to tell the fab what the +/- tolerances are for the holes. At 02:05 AM 10/30/03, you wrote: My question is simple: I want to place a non-plated through hole on my design. I want to void out the plane layers around the hole also. How do I do it? It appears that I can either place a pad or a via, but neither is really a through hole, and it's not obvious (to me, at least) that they will correctly void out the plane layer. Posted from Association web site by: Stuart Brorson snip * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] How to place non-plated thru holes?
Igor Gmitrovic wrote: You can set the pad size as small as you want, even as a negative value. Usually, I set it to 0 (zero) to make sure the pad copper does not show at all. If you want to sort them by size and still don't want copper, set pad sizes to different negative values. Dennis, this is not an attempt to give you the definitive answer. Igor Just for an alternate viewpoint: I like to have a copper pad around mounting holes (and I let them be plated). I make the pad a bit larger than the screwhead or other mounting hardware - this gives me an automatic keepout area around the hole so that I can't run traces where a screwhead might cause a short. The pad doesn't need to be connected to any net. -- Peter Bennett TRIUMF 4004 Wesbrook Mall, Vancouver, BC, Canada GPS and NMEA info and programs: http://vancouver-webpages.com/peter/index.html * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
