[SI-LIST] Re: PCB thickness
- From: Istvan Novak <istvan.novak@xxxxxxxxxxx>
- To: hitheshn@xxxxxxxxx
- Date: Sat, 02 Feb 2013 00:31:00 -0800
Hi Hithesh,
Different fab houses may have access to, or may prefer to use, different
laminates.
With your stackup, however, there seems to be a very simple solution.
Unless
you use L5 and L6 for broadside coupled differential routing, you can
ask the second
fab house to add board thickness by increasing the L3-L4 and L5-L6
thicknesses
by the same amount so that the total board thickness comes closer to
your target.
Regards,
Istvan Novak
Oracle
On 2/2/2013 12:11 AM, Hithesh wrote:
> Hi,
> It's an 8 layer board.
> Stack up below
> L1: Fan out/GND
> L2: GND
> L3: Sig
> L4: PWR
> L5: Sig
> L6: Sig
> L7: GND
> L8: Fan out/GND
>
> The Cu thickness is 1oz on inner layers and 1oz finished thickness on outer
> layers.
> The Er/dielectric is left to the fab house.
> The board has high speed USB diff signals and DDR2 (133MHz).
>
> We use different Fab house for protos and production. The proto Fab house
> did not have any difficulty achieving board thickness and our impedance
> requirement. But the production Fab house wants to reduce PCB thickness and
> modify dielectric thickness.
>
> Regards
> -Hithesh
>
>
> On Sat, Feb 2, 2013 at 1:32 PM, Nobuyuki Kunito <kunito@xxxxxxxxxxx> wrote:
>
>> Hithesh,
>>
>> First of all, please tell us:
>> How many layers the PCB have?
>> Layer construction and/or stack up (the thickness of metal, dielectric
>> material and Er of each dielectric material etc.)
>> I am guessing that the PCB fib house may change the dielectric material..
>>
>> Please give us the information above first.
>>
>> Regards,
>> Nobuyuki Kunito.
>> The president of Debug Lab.
>> http://debuglab.jp
>> (Sorry, Japanese only now. English page will be coming soon)
>>
>> (2013/02/02 15:17), Hithesh wrote:
>>> Hi,
>>> What is the impact of changing PCB thickness?
>>> To cut a long story short, the PCB fab house we use said they can't meet
>>> our impedance requirement and achieve board thickness of 1.6mm.
>>> They have to reduce the board thickness to 1.13mm to meet impedance
>>> requirement.
>>> He did say they could achieve both when we sent them the stack up pdf.
>> But
>>> now they said they can't take decisions just based on stack up.
>>>
>>> Regards
>>> -Hithesh
>>>
>>>
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
Other related posts:
