Maker Pro
Maker Pro

0.031" Thick FR4 PCB

  • Thread starter Darol Klawetter
  • Start date
D

Darol Klawetter

Jan 1, 1970
0
I'm considering using a 0.031" thick FR4 PCB for my next design. What has been your experience with 0.031" PCBs? Have you had durability problems? Did it complicate manufacturing? My PCB will be roughly 3" x 3".

Thanks,

Darol Klawetter
 
S

Spehro Pefhany

Jan 1, 1970
0
I'm considering using a 0.031" thick FR4 PCB for my next design. What has been your experience with 0.031" PCBs? Have you had durability problems? Did it complicate manufacturing? My PCB will be roughly 3" x 3".

Thanks,

Darol Klawetter

Have done 0.02" (2-layer) with no problems.

If your 0.031" board has more than 4 layers it might be an issue.
 
D

Darol Klawetter

Jan 1, 1970
0
Have done 0.02" (2-layer) with no problems.



If your 0.031" board has more than 4 layers it might be an issue.

I'm planning on 6 layers. Stackup is as followins

1 oz Cu
1 Sheet 106, 1 Sheet 1080
1 oz Cu
0.005" Core
1 oz Cu
1 Sheet 106, 1 Sheet 1080
1 oz Cu
0.005" Core
1 oz Cu
1 Sheet 106, 1 Sheet 1080
1 oz Cu
 
J

Jamie

Jan 1, 1970
0
Darol said:
I'm considering using a 0.031" thick FR4 PCB for my next design. What has been your experience with 0.031" PCBs? Have you had durability problems? Did it complicate manufacturing? My PCB will be roughly 3" x 3".

Thanks,

Darol Klawetter

That's a nice size but one time we got carried away and forgot to
check the rail specs a extruded aluminum chassis's we had already
purchased, had to machine them a little to get the boards in.

If you don't have any problem there then thickness shouldn't a
factor.

We visited a tyco facility once, watched them do some 64 layer
boards but I guess that isn't the limit, but it sure was interesting to
say the least.

Jamie
 
  That's a nice size but one time we got carried away and forgot to
check the rail specs a extruded aluminum chassis's we had already
purchased, had to machine them a little to get the boards in.

   If you don't have any problem there then thickness shouldn't a
factor.

   We visited a tyco facility once, watched them do some 64 layer
boards but I guess that isn't the limit, but it sure was interesting to
say the least.

Jamie

we do 10 layers in ~1.5mm (~0.06")

board thickness put a limit on via and hole sizes, thicker board and
the holes need to be bigger

-Lasse
 
we do 10 layers in ~1.5mm (~0.06")

board thickness put a limit on via and hole sizes, thicker board and
the holes need to be bigger

Yep. That's the reason we're starting to go to less than 1.5mm (1mm,
IIRC) boards; can't do the vias on .5mm BGAs. Don't know that we're
going to actually do any products with .5mm BGAs but we need them for
prototypes.
 
Yep.  That's the reason we're starting to go to less than 1.5mm (1mm,
IIRC)  boards; can't do the vias on .5mm BGAs.  Don't know that we're
going to actually do any products with .5mm BGAs but we need them for
prototypes.

ccould do blind/burried vias, the problem is plating deep a shallow
hole, vias that only go through part of the stack shouldn't have that
problem

or maybe via in pad will work

-Lasse
 
R

Robert Baer

Jan 1, 1970
0
Darol said:
I'm considering using a 0.031" thick FR4 PCB for my next design. What has been your experience with 0.031" PCBs? Have you had durability problems? Did it complicate manufacturing? My PCB will be roughly 3" x 3".

Thanks,

Darol Klawetter
I have used PCB material down to 14 mils with no problems.
Then again,what i used was equivalent to Getek (Megtron).
To 200C no sweat.
 
J

Jamie

Jan 1, 1970
0
Robert said:
I have used PCB material down to 14 mils with no problems.
Then again,what i used was equivalent to Getek (Megtron).
To 200C no sweat.

We ordered some FR5/G11 recently and it was a task to get it
here in the states in small quantity. But we did manage to get
3/16" thick and sure works well for HV plus structural
strength:)

Jamie
 
T

Tim Williams

Jan 1, 1970
0
Jamie said:
We visited a tyco facility once, watched them do some 64 layer
boards but I guess that isn't the limit, but it sure was interesting to
say the least.

Some day I might build a particularly high performance planar transformer,
using a PCB stack thicker than it is wide.

A number of manufacturers are offering "heavy copper" these days (> 10
oz.), pretty cool.

Tim
 
ccould do blind/burried vias, the problem is plating deep a shallow
hole, vias that only go through part of the stack shouldn't have that
problem

We do some of that, but it's expensive and I don't know if the process
is qualified for production. OTOH, thin boards have their own set of
problems.
or maybe via in pad will work

No, that doesn't solve the l/w limit on vias.
 
I have used PCB material down to 14 mils with no problems.
Then again,what i used was equivalent to Getek (Megtron).
To 200C no sweat.

I've seen 1 and 2 mil FR4. It makes a pretty nice flex circuit,
better than kapton in many ways.
 
We do some of that, but it's expensive and I don't know if the process
is qualified for production.  OTOH, thin boards have their own set of
problems.


No, that doesn't solve the l/w limit on vias.

it doesn't solve the l/w limit, but it may be possible to route
with the bigger vias when you have the vias in the pad and don't
need to fit them between the pads

-Lasse
 
B

Boris Mohar

Jan 1, 1970
0
No problems here.

The only issue I had was with small panelized boards. The panel was scored
but the gorilla that separated them managed to induce invisible cracks in
ceramic caps near the edges. On the next run I re scored the boards and
separated them without flexing.
 
The only issue I had was with small panelized boards. The panel was scored
but the gorilla that separated them managed to induce invisible cracks in
ceramic caps near the edges. On the next run I re scored the boards and
separated them without flexing.

At the PPoE they had problems with traces cracking after panel
separation. The solution was deeper scoring and larger mouse bites.
Make sure there is a decent setback for any planes or signal traces,
as well.
 
F

Fred Bartoli

Jan 1, 1970
0
[email protected] a écrit :
At the PPoE they had problems with traces cracking after panel
separation. The solution was deeper scoring and larger mouse bites.
Make sure there is a decent setback for any planes or signal traces,
as well.

I have a small board (8mm dia) that's top&bottom stuffed with 0402,
0201, uBGA,... and we also needed some accuracy on the max board diameter.

Usual separation was... scary, at least, so we ended to laser cut them:
fast, accurate, no strain. What's more to be desired? Ah, yes, low cost...
 
T

Tim Williams

Jan 1, 1970
0
Boris Mohar said:
The only issue I had was with small panelized boards. The panel was
scored
but the gorilla that separated them managed to induce invisible cracks
in
ceramic caps near the edges. On the next run I re scored the boards and
separated them without flexing.

Good practice anyway to place chip components perpendicular to nearby
sources of strain, in this case, parallel to the board edge. That's what
the manufacturers recommend. May not be enough though, given the presence
of said gorillas.

I like routed/milled boards better anyway: you don't get fingers full of
itchy fibers from handling them :)

Tim
 
How about snapping them over the edge of some 'Die Knife', like they
use to make cuts in cardboard boxes? It comes in long strips and is
sheared to length, then a thin router bit cuts a groove into plywood to
hold it. A rubber mallet is used to tap it into place. Ad an adjustable
backstop with a lip to keep the board level will help you align the
score on the sharp edge & snap it off without spreading all the stress
through the boards.

It's tough to do with components on both sides of the board, on both
sides of the score. There are tools to do this but they were too
cheap (but wasted *tons* in other areas). The problem is that the
recommended score and mouse bites are marginal, and of course everyone
crowds the edges (raises hand). "I *know* that ten pounds will fit in
that 5# bag."
I don't have any scraps left, but any company that makes the dies for
cutting cardboard boxes will have some. A lot of box companies do it in
house. Every plant I was ever in had the tools & supplies to make &
repair the dies.

I would think you'd need a different tool for each board. Several, in
fact. Once we got the recipe down, there weren't a lot of problems.
The problems were up-front, when the schedules are the tightest, of
course (get the thing to market so the boss can afford to pay us).
 
Eventually the impedances get to be impossible. If the dielectrics are
thin enough, you can't fab a 50 ohm trace any more.

In the ECL mainframe days, 80ohms was the normal trace impedance (some
used 50 ohms for clocks). The higher impedance reduced power, at the
cost of speed, of course (which is why the clocks were often 50 ohm).
When I designed the testers, I usually chose 90 ohms; lower current
yet and it's close to ribbon cable (~100 ohms).
 
In the ECL mainframe days, 80ohms was the normal trace impedance (some
used 50 ohms for clocks).  The higher impedance reduced power, at the
cost of speed, of course (which is why the clocks were often 50 ohm).
When I designed the testers, I usually chose 90 ohms; lower current
yet and it's close to ribbon cable (~100 ohms).

the problem is in the other direction, when you get very
thin dielectric you can't make a trace that is thin enough
to get up to 50R


-Lasse
 
Top