Multilayer PCB Notes.

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

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

So how do you spec the required flatness? I've only seen problems after soldering.

Best regards, Spehro Pefhany

--
"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.

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

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

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

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

Error 500. Access from here:

You can download the pdf after you look at their Donations page.

You probably have this covered, but there's a basic checklist at the end of the PCB design tutorial here:

-Tom

--

To respond by email, replace "somewhere" with "astro" in the
return address.

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

GMM50 wrote:

PCB

bare

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

. 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.

-- Sincerely, Brad Velander

number and color

to specify.

nor should

out before.

or whichever

give a sensible

for it. A

PCB

bare

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