Thanks Veronika,
for providing me with a safe number and a recommended number for my 1700V
clearance.
I would still like to learn how to derive that number for myself.
but thanks,
Jack
On Fri, Jun 20, 2014 at 12:39 PM, Anderson, Veronika <
[log in to unmask]> wrote:
> You will be safe with 6mils min for 1700V. I would design to 8 mil
> separation. It will allow a use multi ply core and prepreg.
>
> Veronika Anderson C.I.D | Sr. Electrical/Mechanical Design Engineer |
> Excelitas Technologies
>
> Office: +1 626.967.9521 x 236
> 1330 East Cypress Street, Covina, CA 91724 USA
> [log in to unmask]
> www.excelitas.com
>
> -----Original Message-----
> From: DesignerCouncil [mailto:[log in to unmask]] On Behalf Of Jack
> Olson
> Sent: Friday, June 20, 2014 8:55 AM
> To: [log in to unmask]
> Subject: Re: [DC] z-axis separation for high voltage
>
> Thanks for taking the time to respond (and to everyone else who responded
> too), and I understand your point about derating, but I am more focused on
> the STARTING clearance for 1700V,
>
> IPC Table 6-1 gives me something slightly over 125 mils, and my board is
> only 62 mil thickness, about half!
> I wasn't initially worried
> because if you look at the slash sheets for dielectric material, its more
> in the KV range PER MIL but now I'm starting to wonder...
>
> Where can I learn more about this?
>
>
> On Fri, Jun 20, 2014 at 10:45 AM, Joel S. Peiffer <[log in to unmask]>
> wrote:
>
> > William provides some good advice to derate the materials insulation
> > resistance significantly as well as providing some of the reasons for
> > doing this (copper surface roughness, dielectric defects).
> >
> > I would like to go into a little more detail on derating. The boards
> > operating conditions (temp, humidity) and expected service life need
> > to be taken into account as well. High temp/humidity operating
> > environments may call for additional derating. The overlap area of
> > high voltage should also be taken into consideration. If the area is
> > very small, the likelihood of a material defect is very small.
> > However, if the area is very large, the likelihood of a material
> > defect will increase in proportion to the area and the material may
> > have to be derated appropriately. Finally, the derating should be
> > dependent on the dielectric thickness. Thus, thicker materials need
> > to be derated less than thinner materials. For example, a 0.5 mil
> > defect may not have much impact on a 5 mil thick material but it will
> > have severe consequences on a
> > 1 mil thick material.
> >
> > If you need to utilize very thin dielectrics to ensure you meet you z
> > axis thickness requirements, you may want to look at materials other
> > than FR-4 to provide the required insulation resistance requirements.
> > Some of the polyimide film materials have excellent insulation
> > resistance and may be a better choice in this situation.
> >
> > Regards, Joel
> >
> >
> > Joel S. Peiffer
> > 3M Electronic Materials Solutions Division 3M Center, Building
> > 201-1E-17 St. Paul, MN 55144
> > Tel: (651) 575-1464
> > Cell: (612) 327-1983
> > [log in to unmask]
> >
> >
> >
> > From: "Brooks, William" <[log in to unmask]>
> > To: <[log in to unmask]>
> > Date: 06/20/2014 10:11 AM
> > Subject: Re: [DC] z-axis separation for high voltage
> > Sent by: DesignerCouncil <[log in to unmask]>
> >
> >
> >
> > The epoxy/glass dielectric actually is spec'd at 750V per mil
> > insulation resistance perpendicular to the layers according to
> > Mil-P-13949/4C for FR4 glass epoxy laminated materials. So 1.3 mils
> > minimum of material perpendicular to the layers would net you 1KV
> > insulation resistance top to bottom or internal layer to layer.
> >
> > Always give yourself some margin... The back side of the copper foil
> > is rough and can be 'spiked' on the laminated side for foil
> > adhesion... those spikes can cause the spacing to be less than the
> > minimum target spacing you require when laminated. Also there can be
> > bubbles or voids in the materials that could occur right between your
> > two high voltage conductors... Unless you are trying to mimic a
> > capacitance plane pair, there is little or no reason to have the high
> voltage lines that close.
> > You don't want a short to occur internally in the board. Give yourself
> > a buffer of at least a couple of additional layers of 2 mil prepreg on
> > internal layers. Just saying... :) Good design practice is to de-rate
> > by 50%.
> >
> > I don't warranty sharing my observations... or advice... but if you
> > feel the need to compensate me... I like microbrewery beers... the
> > Darker Belgian style... I'm not a big hops lover... though I like the
> > hoppy beers too just not as much... :)
> >
> >
> > William Brooks, CID+
> > Senior MTS (Contract)
> > 2747 Loker Ave West
> > Carlsbad, CA 92010-6603
> > 760-930-7212
> > Fax: 760.918.8332
> > Mobile: 760.216.0170
> > E-mail: [log in to unmask]
> >
> >
> >
> > -----Original Message-----
> > From: DesignerCouncil [mailto:[log in to unmask]] On Behalf Of
> > Jack Olson
> > Sent: Friday, June 20, 2014 7:35 AM
> > To: [log in to unmask]
> > Subject: [DC] z-axis separation for high voltage
> >
> > maybe I'm having a "not enough coffee yet" morning, but I was asked
> > how much separation I need between layers for high voltage.
> >
> > We have a design that may have 1700V in several places.
> > Since we are looking at a clearance into the board, layer-to-layer I'm
> > pretty sure I can use the "internal" column B1 of Table 6-1 in
> > IPC-2221 (using Table 6-1 for z-axis was discussed in a committee
> > meeting and no one
> > disagreed)
> >
> > but the number I get for 1700V is =
> > (.25 mm for the first 500V) plus (.0025 mm for each of the other
> > 1200V, 3
> > mm)
> > equals 3.25 mm
> >
> > For one thing, it already seems like I'm off-track because .25 for
> > 500V doesn't correspond very well with 3 mm for 1200V, but if you
> > can't trust IPC..... well, let's not go there.
> >
> > My REAL question is that, although I'm safe using 3.25 mm, my board is
> > not that thick!
> > Is there a smaller z-axis clearance that can be used for 1700V? across
> > typical FR4 material?
> > (we are using a RoHS compatible 170Tg /126)
> >
> > What's the MINIMUM layer spacing I can use for 1700V?
> >
> > thanks,
> > Jack
> >
> >
>
______________________________________________________________________
This email has been scanned by the Symantec Email Security.cloud service.
For more information please contact helpdesk at x2960 or [log in to unmask]
______________________________________________________________________
---------------------------------------------------------------------------------
DesignerCouncil Mail List provided as a free service by IPC using LISTSERV 16.0.
To unsubscribe, send a message to [log in to unmask] with following text in
the BODY (NOT the subject field): SIGNOFF DesignerCouncil.
To temporarily stop/(restart) delivery of DesignerCouncil send: SET DesignerCouncil NOMAIL/(MAIL)
For additional information, or contact Keach Sasamori at [log in to unmask] or 847-615-7100 ext.2815
---------------------------------------------------------------------------------
|
