Is this 4-layer PCB good for mains?

[Piotr Wyderski]

Here is the default stackup 4-layer PCB offered by a Chinese manufacturer:

https://www.allpcb.com/4_layer_pcb.html

The stackup is drawn at the very top, the specification of the
thickneses is at the bottom. Whould it be OK to use it in a 3-phase
400V AC system if all the layers would carry the mains potential?
The core (layers 2 and 3) would suffice for sure, but how about the
internal to top/bottom layers? Can prepreg be trusted enough? And
even if so, can it lead to any EU/US regulations violation?

Best regards, Piotr

 

On Sun, 11 Aug 2019 11:18:57 +0200, Piotr Wyderski
<peter.pan@neverland.mil> wrote:

Here is the default stackup 4-layer PCB offered by a Chinese manufacturer:

https://www.allpcb.com/4_layer_pcb.html

The stackup is drawn at the very top, the specification of the
thickneses is at the bottom. Whould it be OK to use it in a 3-phase
400V AC system if all the layers would carry the mains potential?
The core (layers 2 and 3) would suffice for sure, but how about the
internal to top/bottom layers? Can prepreg be trusted enough? And
even if so, can it lead to any EU/US regulations violation?

Does it say somewhere in the specification that it can handle 2500 V
or just 1500 V between layers ?

Those are the peak voltages that should be expected in mains
electricity.

Some requirements might require such test voltages for a minute.

 

[Tim Williams]

<upsidedown@downunder.com> wrote in message
news:j6qvkedbptr9dr2ohfqbb7d92ivgp7cbbi@4ax.com...

Does it say somewhere in the specification that it can handle 2500 V
or just 1500 V between layers ?

More like 4kV for industrial mains. Unless you've got a surge protector
upstream of this.

Typical breakdown (or maybe minimum?) 20kV/mm, so I wouldn't recommend it.

Personally I've seen 650V across a 7 mil internal gap, which survived most
of the time (testing of several protos), but one article did fail shorted.

Could also order a 6-layer proto and ignore the mid top/bottom. Unless the
middle layers are too close together. Those might not be proto though.
Custom boards aren't expensive in any case.

Tim

--
Seven Transistor Labs, LLC
Electrical Engineering Consultation and Design
Website: https://www.seventransistorlabs.com/

 

[piglet]

On 11/08/2019 10:18 am, Piotr Wyderski wrote:

Here is the default stackup 4-layer PCB offered by a Chinese manufacturer:

https://www.allpcb.com/4_layer_pcb.html

The stackup is drawn at the very top, the specification of the
thickneses is at the bottom. Whould it be OK to use it in a 3-phase
400V AC system if all the layers would carry the mains potential?
The core (layers 2 and 3) would suffice for sure, but how about the
internal to top/bottom layers? Can prepreg be trusted enough? And
even if so, can it lead to any EU/US regulations violation?

    Best regards, Piotr

Just goes to show you need to check each fab's stackup - mine for a 4
layer has 1-2 and 3-4 with fr4 cores and prepreg between layers 2-3.

Personally I wouldn't trust prepreg above 60V for sustained periods.

piglet

 

[Lasse Langwadt Christense]

søndag den 11. august 2019 kl. 20.47.14 UTC+2 skrev Rick C:

On Sunday, August 11, 2019 at 2:22:54 PM UTC-4, piglet wrote:
On 11/08/2019 10:18 am, Piotr Wyderski wrote:
Here is the default stackup 4-layer PCB offered by a Chinese manufacturer:

https://www.allpcb.com/4_layer_pcb.html

The stackup is drawn at the very top, the specification of the
thickneses is at the bottom. Whould it be OK to use it in a 3-phase
400V AC system if all the layers would carry the mains potential?
The core (layers 2 and 3) would suffice for sure, but how about the
internal to top/bottom layers? Can prepreg be trusted enough? And
even if so, can it lead to any EU/US regulations violation?

    Best regards, Piotr

Just goes to show you need to check each fab's stackup - mine for a 4
layer has 1-2 and 3-4 with fr4 cores and prepreg between layers 2-3.

I'm unclear how they can have copper on top and bottom over prepreg. Core comes with copper already on both sides, that's why it would normally be core-prepreg-core rather than prepreg-core-prepreg.

I'm wondering if they actually are showing a correct stackup.

I suppose they could plate the prepreg the same way they plate vias, but why bother with that? It has to be easier to just use two layers of core and one prepreg.

https://www.pcbway.com/pcb_prototype/Cost_cores_Foil___Prepreg_for_PCBs.html

"
3. Copper foils
The copper for the outer layers of multilayer boards is applied in the form of copper foil and pressed together with the prepregs / cores. PCBWay have copper foil of 35Îźm and 70Îźm in stock.
"

 

[Rick C]

On Sunday, August 11, 2019 at 2:22:54 PM UTC-4, piglet wrote:

On 11/08/2019 10:18 am, Piotr Wyderski wrote:
Here is the default stackup 4-layer PCB offered by a Chinese manufacturer:

https://www.allpcb.com/4_layer_pcb.html

The stackup is drawn at the very top, the specification of the
thickneses is at the bottom. Whould it be OK to use it in a 3-phase
400V AC system if all the layers would carry the mains potential?
The core (layers 2 and 3) would suffice for sure, but how about the
internal to top/bottom layers? Can prepreg be trusted enough? And
even if so, can it lead to any EU/US regulations violation?

    Best regards, Piotr

Just goes to show you need to check each fab's stackup - mine for a 4
layer has 1-2 and 3-4 with fr4 cores and prepreg between layers 2-3.

I'm unclear how they can have copper on top and bottom over prepreg. Core comes with copper already on both sides, that's why it would normally be core-prepreg-core rather than prepreg-core-prepreg.

I'm wondering if they actually are showing a correct stackup.

I suppose they could plate the prepreg the same way they plate vias, but why bother with that? It has to be easier to just use two layers of core and one prepreg.

--

Rick C.

- Get 1,000 miles of free Supercharging
- Tesla referral code - https://ts.la/richard11209

 

[Rick C]

On Sunday, August 11, 2019 at 3:12:23 PM UTC-4, Lasse Langwadt Christensen wrote:

søndag den 11. august 2019 kl. 20.47.14 UTC+2 skrev Rick C:
On Sunday, August 11, 2019 at 2:22:54 PM UTC-4, piglet wrote:
On 11/08/2019 10:18 am, Piotr Wyderski wrote:
Here is the default stackup 4-layer PCB offered by a Chinese manufacturer:

https://www.allpcb.com/4_layer_pcb.html

The stackup is drawn at the very top, the specification of the
thickneses is at the bottom. Whould it be OK to use it in a 3-phase
400V AC system if all the layers would carry the mains potential?
The core (layers 2 and 3) would suffice for sure, but how about the
internal to top/bottom layers? Can prepreg be trusted enough? And
even if so, can it lead to any EU/US regulations violation?

    Best regards, Piotr

Just goes to show you need to check each fab's stackup - mine for a 4
layer has 1-2 and 3-4 with fr4 cores and prepreg between layers 2-3.

I'm unclear how they can have copper on top and bottom over prepreg. Core comes with copper already on both sides, that's why it would normally be core-prepreg-core rather than prepreg-core-prepreg.

I'm wondering if they actually are showing a correct stackup.

I suppose they could plate the prepreg the same way they plate vias, but why bother with that? It has to be easier to just use two layers of core and one prepreg.


https://www.pcbway.com/pcb_prototype/Cost_cores_Foil___Prepreg_for_PCBs.html

"
3. Copper foils
The copper for the outer layers of multilayer boards is applied in the form of copper foil and pressed together with the prepregs / cores. PCBWay have copper foil of 35Îźm and 70Îźm in stock.
"

I guess it seems odd to me they would want the extra effort of doing that rather than just using two cores. I suppose they etch two boards either way.. A core and the final stackup or two cores. This particular stack up gives pairs of layers that are very thinly spaced which is good for power plane coupling, but not so good for impedance control unless you work with rather fine trace width as the impedance is controlled by the ratio of trace width to dielectric height. I believe most useful impedances will require rather fine traces if you aren't already using them.

My present board is six layer and I had a bit of back and forth with the PCB house to get the inner layer spacing as thin as I wanted as it is not so easy to make the core layers thin. The board is not very large and I wanted it to have as much inter-plane capacitance as possible. To do that with this stackup would require power/gnd on layers 1 and 2 or 3 and 4 since 2/3 layers are 45 mil spaced.

--

Rick C.

+ Get 1,000 miles of free Supercharging
+ Tesla referral code - https://ts.la/richard11209

 

[Lasse Langwadt Christense]

søndag den 11. august 2019 kl. 22.19.26 UTC+2 skrev Rick C:

On Sunday, August 11, 2019 at 3:12:23 PM UTC-4, Lasse Langwadt Christensen wrote:
søndag den 11. august 2019 kl. 20.47.14 UTC+2 skrev Rick C:
On Sunday, August 11, 2019 at 2:22:54 PM UTC-4, piglet wrote:
On 11/08/2019 10:18 am, Piotr Wyderski wrote:
Here is the default stackup 4-layer PCB offered by a Chinese manufacturer:

https://www.allpcb.com/4_layer_pcb.html

The stackup is drawn at the very top, the specification of the
thickneses is at the bottom. Whould it be OK to use it in a 3-phase
400V AC system if all the layers would carry the mains potential?
The core (layers 2 and 3) would suffice for sure, but how about the
internal to top/bottom layers? Can prepreg be trusted enough? And
even if so, can it lead to any EU/US regulations violation?

    Best regards, Piotr

Just goes to show you need to check each fab's stackup - mine for a 4
layer has 1-2 and 3-4 with fr4 cores and prepreg between layers 2-3..

I'm unclear how they can have copper on top and bottom over prepreg. Core comes with copper already on both sides, that's why it would normally be core-prepreg-core rather than prepreg-core-prepreg.

I'm wondering if they actually are showing a correct stackup.

I suppose they could plate the prepreg the same way they plate vias, but why bother with that? It has to be easier to just use two layers of core and one prepreg.


https://www.pcbway.com/pcb_prototype/Cost_cores_Foil___Prepreg_for_PCBs..html

"
3. Copper foils
The copper for the outer layers of multilayer boards is applied in the form of copper foil and pressed together with the prepregs / cores. PCBWay have copper foil of 35Îźm and 70Îźm in stock.
"

I guess it seems odd to me they would want the extra effort of doing that rather than just using two cores. I suppose they etch two boards either way. A core and the final stackup or two cores.

it also mean they can make boards with thicker copper on the outside layers
without extra plating

 

On Sunday, 11 August 2019 14:25:11 UTC+2, Tim Williams wrote:

upsidedown@downunder.com> wrote in message
news:j6qvkedbptr9dr2ohfqbb7d92ivgp7cbbi@4ax.com...
Does it say somewhere in the specification that it can handle 2500 V
or just 1500 V between layers ?


More like 4kV for industrial mains. Unless you've got a surge protector
upstream of this.

Typical breakdown (or maybe minimum?) 20kV/mm, so I wouldn't recommend it.

Personally I've seen 650V across a 7 mil internal gap, which survived most
of the time (testing of several protos), but one article did fail shorted.

Could also order a 6-layer proto and ignore the mid top/bottom. Unless the
middle layers are too close together. Those might not be proto though.
Custom boards aren't expensive in any case.

We have never seen problems in 3 phase designs

IPC-4101 defines tests for PCBs which manufactors needs to comply with.

For FR-4, it is listed as 40kV/0.78mm, which is close to 50kV/mm

OP has 1kV at 0.18mm, which is about 6kV/mm, so many factors below the test limits

Cheers

Klaus

 

[Tim Williams]

<klaus.kragelund@gmail.com> wrote in message
news:6581290f-bd69-4083-b231-770edf1d88f8@googlegroups.com...
> IPC-4101 defines tests for PCBs which manufactors needs to comply with.

No one needs to comply with IPC. They are a voluntary, private (industry
organized) group.

If you need it UL or CE certified, order boards fabricated and labeled
accordingly, and have the designs reviewed by whatever certifying body is
responsible (UL, ETL, etc. in the US). Pricey (but so are lawsuits).

Tim

--
Seven Transistor Labs, LLC
Electrical Engineering Consultation and Design
Website: https://www.seventransistorlabs.com/

 

[Mikko OH2HVJ]

"Tim Williams" <tiwill@seventransistorlabs.com> writes:

If you need it UL or CE certified, order boards fabricated and labeled
accordingly, and have the designs reviewed by whatever certifying body
is responsible (UL, ETL, etc. in the US). Pricey (but so are
lawsuits).

This is an interesting one: does any certification body take any
responsibility ? This is a question I started thinking about while
gathering some signatures for an IECEx project.

All I've seen they state that your item was tested against some
standardsor state that your stuff has been found to comply
with the standards.

If the shit hits the fan, do they offer any support at that stage ?
(Not that I'm expecting).

--
mikko

 

On Monday, 12 August 2019 04:07:28 UTC+2, Tim Williams wrote:

klaus.kragelund@gmail.com> wrote in message
news:6581290f-bd69-4083-b231-770edf1d88f8@googlegroups.com...
IPC-4101 defines tests for PCBs which manufactors needs to comply with.

No one needs to comply with IPC. They are a voluntary, private (industry
organized) group.

Yes, I should have worded it differently. In our company we need to comply with IPC and I suspect any not garage firm would do the same ;-)

Cheers

Klaus

 

[Phil Hobbs]

On 8/11/19 2:47 PM, Rick C wrote:

On Sunday, August 11, 2019 at 2:22:54 PM UTC-4, piglet wrote:
On 11/08/2019 10:18 am, Piotr Wyderski wrote:
Here is the default stackup 4-layer PCB offered by a Chinese manufacturer:

https://www.allpcb.com/4_layer_pcb.html

The stackup is drawn at the very top, the specification of the
thickneses is at the bottom. Whould it be OK to use it in a 3-phase
400V AC system if all the layers would carry the mains potential?
The core (layers 2 and 3) would suffice for sure, but how about the
internal to top/bottom layers? Can prepreg be trusted enough? And
even if so, can it lead to any EU/US regulations violation?

    Best regards, Piotr

Just goes to show you need to check each fab's stackup - mine for a 4
layer has 1-2 and 3-4 with fr4 cores and prepreg between layers 2-3.

I'm unclear how they can have copper on top and bottom over prepreg. Core comes with copper already on both sides, that's why it would normally be core-prepreg-core rather than prepreg-core-prepreg.

I'm wondering if they actually are showing a correct stackup.

I suppose they could plate the prepreg the same way they plate vias, but why bother with that? It has to be easier to just use two layers of core and one prepreg.

AFAIK you can't plate the prepreg, or there'll be nothing to glue the
cores together during lamination. Plus the prepreg flows a bit, which
would be tough on the plating.

Cheers

Phil Hobbs

--
Dr Philip C D Hobbs
Principal Consultant
ElectroOptical Innovations LLC / Hobbs ElectroOptics
Optics, Electro-optics, Photonics, Analog Electronics
Briarcliff Manor NY 10510

http://electrooptical.net
https://hobbs-eo.com

 

IEC 62368-1:2014 has the following:

G.13.5 (page 240)

Insulation between conductors on different surfaces
The requirements for insulation on the different layers of a multilayer
board are specified below.
For basic insulation there is no thickness requirement.
Supplementary insulation or reinforced insulation between conductive parts
on different surfaces in double-sided single layer printed circuit boards,
multi-layer printed boards and metal core printed boards, shall either have
a minimum thickness of 0.4mm provided by a single layer or conform with
one of the specifications and pass the relevant tests in Table G.14.

Table G.14 Insulation in printed boards

Spec of insulation | Type tests (a) | Routine tests for electric strength (c)

Two layers of sheet insulating | No | Yes
material including prepreg (b)

Three or more layers of sheet | No | No
insulating material including
prepreg (b)

,,,


a Thermal conditioning of G13.6.2 followed by the electrical strength test
of 5.4.9.1.
b Layers are counted before curing.
c Electric strength testing is carried out on the finished printed board.


5.4.9.1 Test procedure for type testing of solid insulation

....

Unless otherwise specified elsewhere in this standard, the test voltage
for the electric strength of basic insulation, supplementary insulation
or reinforced insulation is the highest value of the following three methods:

....

Table 26 Test voltages for electric strength tests based on transient voltages

Required withstand voltage | Test voltage for basic | Test voltage for
kV peak | or supplementary ins | reinforced ins
| kV peak or d.c.

.33 | .33 | .5
.5 | .5 | .8
.8 | .8 | 1.5
1.5 | 1.5 | 2.5
2.5 | 2.5 | 4.0
4.0 | 4.0 | 6.0
.... etc ...

Table 27 Test voltages for electric strength tests based on peak working voltages

Peak working voltage up to | Test voltage for basic | Test voltage for
kV peak | or supplementary ins | reinforced ins
| kV peak or d.c.

.33 | .43 | .53
.5 | .65 | .8
.8 | 1.04 | 1.28
1.5 | 1.95 | 2.4
2.5 | 3.25 | 4.0
4.0 | 5.2 | 6.4
.... etc ...



Table 28 Test voltages for electric strength tests based on temporary overvoltages

Nominal mains system voltage | Test voltage for basic | Test voltage for
V rms | or supplementary ins | reinforced ins
| kV peak or d.c.

<=250 | 2 | 4
>250, <=600 | 2.5 | 5

John

 

[Piotr Wyderski]

jrwalliker@gmail.com wrote:

Great input, much appreciated!

> For basic insulation there is no thickness requirement.

In this case it is all about reliability. Safety will be implemented by
proper creepage, clearance and slots. 9mm or more. I just don't want the
board to explode and I am not able to route it on 2 layers.

Best regards, Piotr

 

[Piotr Wyderski]

Tim Williams wrote:

More like 4kV for industrial mains.  Unless you've got a surge protector
upstream of this.

There will be a 20kA MOV per phase at the very input, ETFV25K320E4. But
I habitually don't trust MOVs.

Personally I've seen 650V across a 7 mil internal gap, which survived
most of the time (testing of several protos), but one article did fail
shorted.

This is my primary concern. And the manufacturer doesn't want to tell if
they are willing to make a 2- or 3-layer thick prepreg stackup. After a
lot of
googling I am basically where I started -- custom stackup and proto
quantities don't come tohether.

> Could also order a 6-layer proto and ignore the mid top/bottom.

According to their stackup specification, the outermost layers in
6-layer PCBs are separated by a prepreg, not core, so it would
effectively mean 4 layers with double prepreg. Technically exacty what I
want, but psychologically an overkill. Just give me 2 prepregs and call
it a 4-layer board. ;-)

Best regards, Piotr

 

[Piotr Wyderski]

Rick C wrote:

> Not following what you mean. A 6 layer stack up is two cores and three prepregs. The 4 layer board is one core with the outer most copper layers separated by prepreg.

You are 100% correct here, I didn't pay enough attention to their
6-layer specification and assumed they are just gluing as many
prepreg-foil pairs as needed to the internal core. This is not the case,
thanks.

If you can use a 4 layer board, why would you even be considering a 6
layer board? What am I missing?

The structure of a 4-layer one combined with the unlimited current
capabilities of mains scares me off. This is not about routing
complexity, but about getting sufficient dieelectric strength.
The 6-layer "signal" one would make a decent 3-layer "power" board due
to the presence of 2 cores (connect layer 1-2, 3-4 and 5-6). The 4-layer
board would suffice, but should preferably have double prepreg layers in
order to increase the breakdown voltage and handle prepreg voids.

Best regards, Piotr

 

[Phil Hobbs]

On 8/13/19 7:02 PM, Rick C wrote:

On Tuesday, August 13, 2019 at 6:16:50 PM UTC-4, Piotr Wyderski wrote:

According to their stackup specification, the outermost layers in
6-layer PCBs are separated by a prepreg, not core, so it would
effectively mean 4 layers with double prepreg. Technically exacty what I
want, but psychologically an overkill. Just give me 2 prepregs and call
it a 4-layer board. ;-)

Not following what you mean. A 6 layer stack up is two cores and three prepregs. The 4 layer board is one core with the outer most copper layers separated by prepreg. What's wrong with that? If you can use a 4 layer board, why would you even be considering a 6 layer board? What am I missing?

The four layer boards we use are two cores and one prepreg.

Cheers

Phil Hobbs

--
Dr Philip C D Hobbs
Principal Consultant
ElectroOptical Innovations LLC / Hobbs ElectroOptics
Optics, Electro-optics, Photonics, Analog Electronics
Briarcliff Manor NY 10510

http://electrooptical.net
http://hobbs-eo.com

 

[Rick C]

On Tuesday, August 13, 2019 at 6:16:50 PM UTC-4, Piotr Wyderski wrote:

According to their stackup specification, the outermost layers in
6-layer PCBs are separated by a prepreg, not core, so it would
effectively mean 4 layers with double prepreg. Technically exacty what I
want, but psychologically an overkill. Just give me 2 prepregs and call
it a 4-layer board. ;-)

Not following what you mean. A 6 layer stack up is two cores and three prepregs. The 4 layer board is one core with the outer most copper layers separated by prepreg. What's wrong with that? If you can use a 4 layer board, why would you even be considering a 6 layer board? What am I missing?

--

Rick C.

-- Get 1,000 miles of free Supercharging
-- Tesla referral code - https://ts.la/richard11209

 

[Rick C]

On Tuesday, August 13, 2019 at 7:21:16 PM UTC-4, Phil Hobbs wrote:

On 8/13/19 7:02 PM, Rick C wrote:
On Tuesday, August 13, 2019 at 6:16:50 PM UTC-4, Piotr Wyderski wrote:

According to their stackup specification, the outermost layers in
6-layer PCBs are separated by a prepreg, not core, so it would
effectively mean 4 layers with double prepreg. Technically exacty what I
want, but psychologically an overkill. Just give me 2 prepregs and call
it a 4-layer board. ;-)

Not following what you mean. A 6 layer stack up is two cores and three prepregs. The 4 layer board is one core with the outer most copper layers separated by prepreg. What's wrong with that? If you can use a 4 layer board, why would you even be considering a 6 layer board? What am I missing?


The four layer boards we use are two cores and one prepreg.

That's what I'm accustomed to as well, but I still don't understand your comment "Just give me 2 prepregs and call it a 4-layer board."

--

Rick C.

-+ Get 1,000 miles of free Supercharging
-+ Tesla referral code - https://ts.la/richard11209