[PEDA] Transparent footprints
Hi, I hope you all had a happy Xmas. I need to place two large components on a pcb that will actually be on spacers and connected to the main board by short wire links. As the items are relatively large (one of them is one of those standard 2- or 4-line LCD modules) the footprint for these will be quite large yet be basically empty - there will be four spacers, one for each corner, plus a short multi-way connector. Is there any way of creating this as a component footprint so that it may be correctly moved and position on the main board yet still allow Protel to freely place components and tracks in the free area under these components? As the position of the spacers relative to the connector is fairly critical it is preferable that this is one single component. Best Regards Laurie Biddulph http://www.elby-designs.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Transparent footprints
At 17:33 05.01.2004 +1100, you wrote: Hi, I hope you all had a happy Xmas. I need to place two large components on a pcb that will actually be on spacers and connected to the main board by short wire links. As the items are relatively large (one of them is one of those standard 2- or 4-line LCD modules) the footprint for these will be quite large yet be basically empty - there will be four spacers, one for each corner, plus a short multi-way connector. Is there any way of creating this as a component footprint so that it may be correctly moved and position on the main board yet still allow Protel to freely place components and tracks in the free area under these components? You can place components and tracks under any footprint if you have turned off the Comonent Clearence Constraint design rule. It's just a bit painful to move components under the large components. Every time you pick a component, Protel shows a list to ask which component you wish to move. The way I have done exactly the same thing: - placed the Display footprint - placed four free pads and one connector exactly over the spacers and the connector - looked these five items - deleted the footprint If the position of the display is fixed when you start with the desing, it has to be done only once. A bit cumbersome, bit makes the placing of the other components much easier. Can't think of an easier way at the moment. Edi As the position of the spacers relative to the connector is fairly critical it is preferable that this is one single component. Best Regards Laurie Biddulph http://www.elby-designs.com + IH electronic+ Phone: ++41 52 320 90 00 + + Edi Im Hof + Fax: ++41 52 320 90 04 + + Doernlerstrasse 1, Sulz + URL: http://www.ihe.ch + + CH-8544 Rickenbach-Attikon + E-Mail: [EMAIL PROTECTED] + + Switzerland + + * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Transparent footprints
This can be a bit of a problem. I get around it usually by creating TWO components - one of them just the connector pads with a clearly defined origin on mech or top overlay and the other being the printable outline, on a mech layer or top overlay as you please, that gives you the perspective you need for design or manufacturing purposes. This strategy allows you to plant the full outline as a 'last stage' job to completing the PCB. Of course you could just switch OFF component clearance DRC (do it all the time myself) ... this check feature can be useful on simple boards but is usually too aggressive (translates to 'primitive') for my liking. This is another way of reclaiming the sort of control old blokes like me were accustomed to having in the Bishop Graphics days. Don't get me wrong - wouldn't go back THERE for anything. Happy new Year Jim - Original Message - From: Laurie Biddulph [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] Sent: Monday, January 05, 2004 7:33 PM Subject: [PEDA] Transparent footprints Hi, I hope you all had a happy Xmas. I need to place two large components on a pcb that will actually be on spacers and connected to the main board by short wire links. As the items are relatively large (one of them is one of those standard 2- or 4-line LCD modules) the footprint for these will be quite large yet be basically empty - there will be four spacers, one for each corner, plus a short multi-way connector. Is there any way of creating this as a component footprint so that it may be correctly moved and position on the main board yet still allow Protel to freely place components and tracks in the free area under these components? As the position of the spacers relative to the connector is fairly critical it is preferable that this is one single component. Best Regards Laurie Biddulph http://www.elby-designs.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Transparent footprints
In a message dated 1/5/2004 2:40:04 AM Eastern Standard Time, [EMAIL PROTECTED] writes: I need to place two large components on a pcb that will actually be on spacers and connected to the main board by short wire links. As the items are relatively large (one of them is one of those standard 2- or 4-line LCD modules) the footprint for these will be quite large yet be basically empty - there will be four spacers, one for each corner, plus a short multi-way connector. Is there any way of creating this as a component footprint so that it may be correctly moved and position on the main board yet still allow Protel to freely place components and tracks in the free area under these components? As the position of the spacers relative to the connector is fairly critical it is preferable that this is one single component. I do this sort of thing often. Just build the component normally, using pads for the mounting standoffs. Be sure the pads include holes of the appropriate size, and make the pads large enough to completely contain the hardware (screwhead, nut, washer, etc.) so that you won't have any conflicts electrically. Turn off the component clearance rule; it's so worthless anyway that I always leave it off. I just make sure that my silkscreen outlines include the full IPC clearance areas, and place the components so that the silkscreens touch on a tight design. But the Protel component clearance rules are pretty worthless, in my experience. Steve Hendrix * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Transparent footprints
-Original Message- From: Laurie Biddulph [mailto:[EMAIL PROTECTED] Sent: Monday, January 05, 2004 6:33 AM To: Protel EDA Forum Subject: [PEDA] Transparent footprints Hi, I hope you all had a happy Xmas. I need to place two large components on a pcb that will actually be on spacers and connected to the main board by short wire links. As the items are relatively large (one of them is one of those standard 2- or 4-line LCD modules) the footprint for these will be quite large yet be basically empty - there will be four spacers, one for each corner, plus a short multi-way connector. Is there any way of creating this as a component footprint so that it may be correctly moved and position on the main board yet still allow Protel to freely place components and tracks in the free area under these components? As the position of the spacers relative to the connector is fairly critical it is preferable that this is one single component. I believe you ca do this, although component selection within the boundry box of the larger part will be dificult. I also think you will need to turn off component clearance checking between parts otherwise you will get DRC errors for all parts 'under' the larger part as technically it will have 0 clearance. John * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Transparent footprints
Hello again Laurie, It has just occurred to me that I may have been missing the obvious on this one for years. I use customised design rules for all sorts of 'one-off' exceptions in respect to copper. While this facility is darn fiddly to drive, it is actually pretty clever when you figure out what kind of dope the programmer was on at the time of writing. So.. I wonder if you can set up a 'component footprint' specific design rule that allows zero minimum component clearance between itself and all other components. You would probably need to then ensure the connector/mounting pads were given their specific rules that emulated the normal clearance requirements. Never tried this myself but if you give it a go, let me know how you get on. Regards, Jim - Original Message - From: Laurie Biddulph [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] Sent: Monday, January 05, 2004 7:33 PM Subject: [PEDA] Transparent footprints Hi, I hope you all had a happy Xmas. I need to place two large components on a pcb that will actually be on spacers and connected to the main board by short wire links. As the items are relatively large (one of them is one of those standard 2- or 4-line LCD modules) the footprint for these will be quite large yet be basically empty - there will be four spacers, one for each corner, plus a short multi-way connector. Is there any way of creating this as a component footprint so that it may be correctly moved and position on the main board yet still allow Protel to freely place components and tracks in the free area under these components? As the position of the spacers relative to the connector is fairly critical it is preferable that this is one single component. Best Regards Laurie Biddulph http://www.elby-designs.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Transparent footprints
Laurie: I assume you are using 99SE. I stack components like this all the time. IIRC, there is a design rule that allows components to touch. Set that rule to allowed. If you want to enforce that rule for all other components, create a component class (i.e. TouchAllowed) where all components in that class are allowed to touch. Best regards, Ivan Baggett Bagotronix Inc. website: www.bagotronix.com - Original Message - From: Laurie Biddulph [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] Sent: Monday, January 05, 2004 1:33 AM Subject: [PEDA] Transparent footprints Hi, I hope you all had a happy Xmas. I need to place two large components on a pcb that will actually be on spacers and connected to the main board by short wire links. As the items are relatively large (one of them is one of those standard 2- or 4-line LCD modules) the footprint for these will be quite large yet be basically empty - there will be four spacers, one for each corner, plus a short multi-way connector. Is there any way of creating this as a component footprint so that it may be correctly moved and position on the main board yet still allow Protel to freely place components and tracks in the free area under these components? As the position of the spacers relative to the connector is fairly critical it is preferable that this is one single component. Best Regards Laurie Biddulph http://www.elby-designs.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Transparent footprints
Hi Laurie, You could make up the component, place it on the PCB, load your nets, and then Explode the component to free primitives (ToolsConvertExplode Component to Free Primitives). Of course, the next time you go to load the netlist, the nets on the connector will be lost. The other way I'd suggest, is place the spacer holes on the PCB separately, and create a component of the ribbon connector, with the origin of the component in the same position as one of the spacers, so when you plonk the component down, you can align it perfectly using the spacer holes on the PCB. I've used both of these methods in the past, with success. Just my $0.02. TC -Original Message- From: Laurie Biddulph [mailto:[EMAIL PROTECTED] Sent: Monday, 5 January 2004 5:03 PM To: Protel EDA Forum Subject: [PEDA] Transparent footprints Hi, I hope you all had a happy Xmas. I need to place two large components on a pcb that will actually be on spacers and connected to the main board by short wire links. As the items are relatively large (one of them is one of those standard 2- or 4-line LCD modules) the footprint for these will be quite large yet be basically empty - there will be four spacers, one for each corner, plus a short multi-way connector. Is there any way of creating this as a component footprint so that it may be correctly moved and position on the main board yet still allow Protel to freely place components and tracks in the free area under these components? As the position of the spacers relative to the connector is fairly critical it is preferable that this is one single component. Best Regards Laurie Biddulph http://www.elby-designs.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Transparent footprints
05/01/2004 08:41:51, Edi Im Hof [EMAIL PROTECTED] wrote: You can place components and tracks under any footprint if you have turned off the Comonent Clearence Constraint design rule. The component clearance rule is so broken I always have it turned off anyway... It's just a bit painful to move components under the large components. Every time you pick a component, Protel shows a list to ask which component you wish to move. Not if you lock the big component, and set the protect locked objects in tools - preferences - options And, if the big component is so critical, it should be locked, to avoid embarassment later... Some way to convince Protel that I don't want to move those poxy split plane vertices (or the planes themselves) unless I'm on that layer would be very useful, though. Does DXP handle that differently? Less annoyingly? Steve * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] BGA Tenting/Specifications
Can get I a few opinions about how you guys handle BGA components in your layouts? Do you generally tent (using tenting in Protel99SE via properties) the dog-bone vias that branch off of each BGA pad to prevent solder thieving or specify in your specifications to Plug top side vias. There may be other ideas and I'm sure the responses will vary on the assembly methods. Generally I see a reflow then wave on these mixed technology PWA I am prototyping. Thanks in advance. -MB * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] BGA Tenting/Specifications
re SE99 we tent them you want to do this to improve yield then place free pads on bottom side soldermask to allow probing generally i think plugging is to be avoided for various reasons (assuming by 'plugging' we are referring to put some material in the hole) in DXP you can make top and bottom solder masks different from each other Dennis Saputelli Michael Biggs wrote: Can get I a few opinions about how you guys handle BGA components in your layouts? Do you generally tent (using tenting in Protel99SE via properties) the dog-bone vias that branch off of each BGA pad to prevent solder thieving or specify in your specifications to Plug top side vias. There may be other ideas and I'm sure the responses will vary on the assembly methods. Generally I see a reflow then wave on these mixed technology PWA I am prototyping. Thanks in advance. -MB -- ___ Integrated Controls, Inc. Tel: 415-647-0480 EXT 107 2851 21st StreetFax: 415-647-3003 San Francisco, CA 94110 www.integratedcontrolsinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
