 |
 | Home | Contact Us | FAQ | Search & Site Map | Link to Us |
 | Sign In | Join | Other 45 Sites in Network |
| HomeDiscussion GroupsElectronicsBasicsRepairDesignCADComponentsEquipmentElectrical Engineering ElectronicsKB.com Contact UsLink To UsSearch & Site Map |
Electronics Forum / CAD / February 2005Multilayer PCB Notes.
Hello: I'm about to release for manufacturing a 4 layer PCB 1. Top Signal 2. Ground 3. Power 4. Signal The design rules are 8 mil lines and 8 mil spacing. And it's mostly SMT devices. THe board size is 16 x 10 inches. It's been a while since I specified such a complicated (expensive) PCB and my notes are old. My question is where should I look for a set of notes to add to the detail drawing for the board. Specifying itmes such as silk screen, soldermask, solder mask over bare copper, dimensions and warp and twist. And all the other things I forgot. THanks George > Hello: > [quoted text clipped - 16 lines] > copper, dimensions and warp and twist. > And all the other things I forgot. Most manufacturers sort all that stuff out for you, I just supply the Gerbers and they get on with it. The default values with my PCB software work OK. With a big board like that warp and twist might be a problem, I had problems with a four-layer double-eurocard design some years ago from one supplier. Leon > > Hello: > > [quoted text clipped - 25 lines] > > Leon Properly made PCBs will not warp or twist, unless you cycle them over a large temperature range. >> > Hello: >> > [quoted text clipped - 28 lines] > Properly made PCBs will not warp or twist, unless you cycle them over >a large temperature range. So how do you spec the required flatness? I've only seen problems after soldering. Best regards, Spehro Pefhany  Signature"it's the network..." "The Journey is the reward" speff@interlog.com Info for manufacturers: http://www.trexon.com Embedded software/hardware/analog Info for designers: http://www.speff.com > Properly made PCBs will not warp or twist, unless you cycle them over > a large temperature range. I am fighting with myself whether I want to design for 4 layers or 2 layers. Is a 4 layer board supposed to be less likely to twist than a 2 layer board? I want my boards to last long and keep in good shape even that means some more investment. Thank you. vax, 9000 >> Properly made PCBs will not warp or twist, unless you cycle them over >> a large temperature range. [quoted text clipped - 5 lines] > I want my boards to last long and keep in good shape even that means some > more investment. Thank you. Try to have equal amounts of copper on the top and bottom, evenly distributed, with most of the tracks on the top running at right angles to the tracks on the bottom. That should minimise the problem. Leon >> Properly made PCBs will not warp or twist, unless you cycle them over >>a large temperature range. [quoted text clipped - 5 lines] > > vax, 9000 The twisting and warping is mostly due to poor workmanship when they are thermo laminating the boards together. Multilayer boards are etched as individual one and two sided boards using very thin board stock. They are smeared with a thermo setting adhesive, and run through a hot press. If this stage isn't done correctly, you will get a big warp. As I understand it, the key is to making sure that all the boards are evenly, and thoroughly heated when they are in the press. Success, or failure, is entirely in the hands of your board manufacturer. -Chuck >Hello: > [quoted text clipped - 18 lines] >THanks >George This is what I use to use at a company that I worked for. Include it as a readme.txt file with your gerbers. Fabrication Information from Light & Sound Design. PCB Part No: 5689302A-AW PCB Description: Control Panel Assembly Number of Track Layers: 2 Number of Power Planes: 2 PCB Material: FR4 PCB Thickness: 0.062 inch Copper Weight: 1 Oz finished Top Silkscreen: White Bottom Silkscreen: White Solder Mask Both Sides: Liquid photoimagable Minimum Track Width: 0.008 inch Minimum Clearance: 0.007 inch Solder Mask Expansion: 0.0003 inch (radial) Pad Finish: Hot Air Solder Leveling Fabrication Tools: (layer order to be as follows) 5689302A-AW.GTO Top Silkscreen 5689302A-AW.GTS Top Solder Mask 5689302A-AW.GTL Top Layer Copper Tracks 5689302A-AW.GP1 Internal Plane 1 Copper ( v) 5689302A-AW.GP2 Internal Plane Copper (ground) 5689302A-AW.GBL Bottom Layer Copper Tracks 5689302A-AW.GBS Bottom Solder Mask 5689302A-AW.GBO Bottom Silkscreen --------------------------------------------------------------------------- NCDrill File Report For: 5689302A-AW.pcb 31-Dec-2002 12:15:01 --------------------------------------------------------------------------- Layer Pair : TopLayer to BottomLayer ASCII File : NCDrillOutput.TXT EIA File : NCDrillOutput.DRL Tool Hole Size Hole Count Plated Tool Travel --------------------------------------------------------------------------- T1 32mil (0.8128mm) 2 2.29 Inch (58.29 mm) T2 37mil (0.9398mm) 78 16.12 Inch (409.35 mm) T3 55mil (1.397mm) 8 2.16 Inch (54.93 mm) T4 125mil (3.175mm) 2 NPTH 3.64 Inch (92.52 mm) --------------------------------------------------------------------------- Totals 90 24.22 Inch (615.09 mm) Contact: Patrick T. Caezza Phone: (805) 499-XXXX Fax: (805) 499-XXXX That's a good format for a start. Now what about alignment accruacy/tolerance? I used to use +/- 0.005" but I suspect it can be tighter without adding cost. Board dimensions? Could be covered on the fab drawing. Warp and twist. I've seem 0.005" per inch of board dimension measured by holding one corner of the board to a surface plate and measuring the highest point above that surface. With a larger PCB it needs to be flat enough so the pick and place machine can accurately do it's job. There used to be test cupons used to measure solderability (delamination) on multilayer PCB. We would shock the cupon (no prehead and dip in solder pot) and if it delaminated then we would do a proper test (proper preheating). This gave us a margin. I also need to be sure the solder is level enough to keep the placement accuracy. Any one else?? THanks George You probably have this covered, but there's a basic checklist at the end of the PCB design tutorial here: http://alternatezone.com/electronics/pcbdesign.html -Tom SignatureTo respond by email, replace "somewhere" with "astro" in the return address. >a basic checklist at the end of the PCB design tutorial here: >http://alternatezone.com/electronics/pcbdesign.html > Tom Loredo Error 500. Access from here: http://alternatezone.com/electronics/ You can download the pdf after you look at their Donations page. I normally include a Layer Stack-up legend that gives all the information about the board (Copper Thickness, Core Thickness, Prepreg thickness, Solder Mask thickness, etc). --D > Hello: > [quoted text clipped - 18 lines] > THanks > George > I'm about to release for manufacturing a 4 layer PCB > It's been a while since I specified such a complicated [quoted text clipped - 4 lines] > itmes such as silk screen, soldermask, solder mask over > bare copper, dimensions and warp and twist. The items that define the board, such as number of layers, number and color of silkscreen layers, type of soldermask, etc., you will have to specify. But the Quality stuff you should not have to make up yourself, nor should you have to write it all out explicitly. It's all been worked out before. Just write "Boards to be fabricated to meet IPC-A-600G Class 2" or whichever class is appropriate for your situation. (See www.ipc.org . The web site is so hopeless that I can't give a sensible link to the standard itself, you will have to browse or search for it. A printed copy will set you back about $90.) Mathew's comments are good. Regarding the IPC-A-600G spec though I would have a suggestion. Do not list the revision of IPC specs, just use "IPC-A-600", then have a statement in your notes that states to "...use the latest revision of all IPC specifications." Down the road when IPC specs are revised, your notes are not outdated and any IPC spec improvements will be automatically incorporated on your behalf. SignatureSincerely, Brad Velander > The items that define the board, such as number of layers, number and color > of silkscreen layers, type of soldermask, etc., you will have to specify. [quoted text clipped - 7 lines] > link to the standard itself, you will have to browse or search for it. A > printed copy will set you back about $90.) > Hello: > [quoted text clipped - 18 lines] > THanks > George Here's what I've come up with. ------- Notes: 1.) PCB material: (put your material here I'm using FR4) 2.) Fabricate board in accordance with IPC-6012 (latest Revision) Performance class 2. Board acceptability per IPC-A-600 (latest revisi0n) 3.) Unless other wise specified tolerance - +/- 0.005" 4.) HASL finished pads. 5.) (Specify the solder mask here) 6.) (specify the silkscreen here) 7.) Boards will be 100% electrically tested. --------- I ordered a copy of IPC-A-600 and all the requirements I'm interest in are contained in that documents. Thanks to all who add their 2 cents on this one. George |
Reply to this Message |
 Sign In
 Join
 My Latest Posts My Monitored Threads My Blog My Photo Gallery My Profile My Homepage Start New Thread Enable EMail Alerts Rate this Thread
|
©2009 Advenet LLC Privacy Policy - Terms of Use
This website includes both content owned or controlled by Advenet as well as content owned or controlled by third parties.