Thank You! Your info will help me figure this out.
Jeff Adolphs
-----Original Message-----
From: John Haddy [mailto:[EMAIL PROTECTED]]
Sent: Tuesday, July 10, 2001 7:20 PM
To: Protel EDA Forum
Subject: Re: [PEDA] 80 Mil Thick PCB
>From my fabricator's standard build list (which I never use :-):
4 layer, 2.0mm nom. finished thickness; 0.5oz foil construction:
18um Cu foil
3 x 8000 prepreg (0.588mm)
0.71mm core (laminated both sides with 18um Cu) - (0.745mm)
3 x 8000 prepreg (0.588mm)
18um Cu foil
giving an expected thickness range between 1.83mm and 2.04mm, with a
mean of 1.95mm. (Remember to add plating/soldermask/silkscreen
allowances if they'll affect your specific situation)
4 layer, 1.6mm nom. finished thickness; 0.5oz foil construction:
18um Cu foil
2 x 7628 prepreg (0.348mm)
0.71mm core (laminated both sides with 18um Cu) - (0.745mm)
2 x 7628 prepreg (0.348mm)
18um Cu foil
giving an expected thickness range between 1.39mm and 1.57mm, with a
mean of 1.48mm.
Cheers,
John Haddy
> -----Original Message-----
> From: Jeff Adolphs [mailto:[EMAIL PROTECTED]]
> Sent: Wednesday, 11 July 2001 12:12 AM
> To: Protel EDA Forum (E-mail)
> Subject: [PEDA] 80 Mil Thick PCB
>
>
> Hello,
>
> Thanks for all the information in the Layer Stackup Info. string!
>
> Would anyone give me an example of a board stackup (4 layer) for a 80 mil
> thick PCB and a 62 mil thick PCB?
>
> I don't have the IPC standard for prepreg. The PCB is specified as 80 mil
> for mechanical
> reasons only. The PCB is 16" wide x 13" long and with 62 mil thickness the
> board bounces
> in the solder wave process. At 80 mils the PCB is stronger and
> still allows
> the components
> designed for 62 mil thick PCB's to work (components all thru-hole).
>
> Without the board stackup specified sometimes the PCB thickness
> comes in at
> 62 or 90 mil
> instead of what is specified 0.080" +/- 0.006".
>
> Thank You!
> Jeff Adolphs
> Lake Shore Cryotronics, Inc.
> Westerville, Ohio, USA
>
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
* - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
