Multilayer PCB Notes.
GMM50
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
Leon Heller
news:1107402431....@z14g2000cwz.googlegroups.com...
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
Patrick T. Caezza
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
Robert Baer
Properly made PCBs will not warp or twist, unless you cycle them over
a large temperature range.
Spehro Pefhany
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"
sp...@interlog.com Info for manufacturers: http://www.trexon.com
Embedded software/hardware/analog Info for designers: http://www.speff.com
GMM50
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
vax, 9000
> 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
Leon Heller
news:cu719l$qpo$1...@charm.magnus.acs.ohio-state.edu...
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
Chuck Harris
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
Tom Loredo
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
--
To respond by email, replace "somewhere" with "astro" in the
return address.
JeffM
>http://alternatezone.com/electronics/pcbdesign.html
Error 500. Access from here:
http://alternatezone.com/electronics/
You can download the pdf
after you look at their Donations page.
doppan
information about the board (Copper Thickness, Core Thickness, Prepreg
thickness, Solder Mask thickness, etc).
--D
Matthew Kendall
> I'm about to release for manufacturing a 4 layer PCB
> (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.
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 $90.)
Brad Velander
Regarding the IPC-A-600G spec though I would have a
suggestion. Do not list the revision of IPC specs, just use
"IPC-A-600", then have a statement in your notes that states to
"...use the latest revision of all IPC specifications."
Down the road when IPC specs are revised, your notes are not
outdated and any IPC spec improvements will be automatically
incorporated on your behalf.
--
Sincerely,
Brad Velander
"Matthew Kendall" <mdke...@hotmail.com> wrote in message
news:mmVQd.412090$Xk.333420@pd7tw3no...
GMM50
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