From: Greim, Michael ([email protected])
Date: Tue Dec 12 2000 - 08:18:43 PST
If you route the back side of the board in the card
guide area, this is not an issue. However, if you do
this on the side that the connector is mounted on, then
you need to route out the board at the card guide,
connector housing and mounting blocks. This will
maintain your proper alignement with the front panel
and backplane connector.
I have used a compound routing technique in the past
to fit a 130 mil thick board in to VME card guides.
By resolving your congestion and employing back side
card guide routing. You should be able to achieve your
goals and have a reasonable board stackup.
best regards,
Michael Greim
-----Original Message-----
From: Aric Hadav [mailto:[email protected]]
Sent: Tuesday, December 12, 2000 10:57 AM
To: 'e'
Cc: '[email protected]'
Subject: RE: [SI-LIST] : layer stackup
Hi,
the board is connected to a backplane,so if you increase the board
thickness,
the board connectors won't connect to the backplane connectors.
hence - I thought off trimming/cutting the board to 1.6 mm in this side as
well, but doing so
will destroy the connectors pads.
that's why I cannot change the alignment of the board compared to the
backplane
connectors.
I'll be happy to receive any more ideas on the matter.
thanks,
Aric
-----Original Message-----
From: e [mailto:[email protected]]
Sent: Tuesday, December 12, 2000 5:36 PM
To: Aric Hadav
Cc: '[email protected]'; 'Dave Hoover'
Subject: Re: [SI-LIST] : layer stackup
Aric,
Is it possible to add more layers to the board, and so increase the
thickness,
but keep it at 1.6 mm along the edges where it must be inserted into card
guides?
Ellis
Aric Hadav wrote:
> Hi,
>
> board thickness is fixed to 1.6 mm because of card guides.
> I thought of making a wider card and cutting it at the edges to 1.6 mm but
> that makes too many problems, hence I'm staying with 1.6mm.
> regarding the board warpage, the layout guy told me the layout software
(by
> Cadence)
> has a copper balance feature that insures a balanced board by the end of
the
> layout.
> still, I'm not confident with that.
> has anyone has a better stackup in 1.6 mm ? or other ideas ?
>
> thanks,
> Aric
>
> -----Original Message-----
> From: Dave Hoover [mailto:[email protected]]
> Sent: Tuesday, December 12, 2000 4:08 AM
> To: Aric Hadav; '[email protected]'
> Subject: Re: [SI-LIST] : layer stackup
>
> Aric,
> 14 layers in 1.6 mm is tough but possible. It looks
> like your forced to go this way based on necessary
> signal layers. Unfortunately this stackup you've
> proposed is not well balanced. There may be a
> considerate amount of warpage because of this
> unbalanced stackup. Being 1.6mm thk just compounds
> the warpage. Is there any way to add redundant
> planes (to balance the stackup) and increase the
> overall thickness? (Is the thickness locked in due
> to card guides, pressfit pin lengths, or something?)
>
> Dave Hoover (fab guy learning about SI)
>
> --- Aric Hadav <[email protected]> wrote:
> > Hi,
> >
> > I'm looking for some help on deciding on my board
> > layer stackup.
> > my design has ~20K pads and it must fit into a
> > standard 6U board, 1.6 mm
> > thick.
> > the board thickness CAN NOT be changed.
> >
> > the PCB layout guy told me that the design can only
> > fit into a minimum of 14
> > layers stack up,
> > with a 3-4 mil core and preg thickness, as described
> > below:
> > 1. CS
> > 2. sig1
> > 3. VCC1V8
> > 4. sig2
> > 5. sig3 (ctrl impedance).
> > 6. sig4
> > 7. GND
> > 8. sig5
> > 9. sig6 (ctrl impedance).
> > 10. sig7
> > 11. VCC3V
> > 12. sig8
> > 13. sig9
> > 14. PS
> >
> > now, this looks some what strange to me since layers
> > 5 & 9 aren't adjacent
> > to a PWR/GND
> > plane, since one should always try that a signal
> > layer will be close to
> > reference plane.
> > now, in order to reduce the crosstalk between layers
> > 4 to 6 or 8 to 10 he
> > suggested to route the
> > signals not horizontally and vertically but
> > layers 4, 8 - 45 degrees.
> > layers 5, 9 - vertical or horizontal.
> > layers 6, 10 - 135 degrees.
> > has anyone routed this way ? did it work ok ?
> > the signal clocks will be routed in layers 5 and 9
> > which supposed to be
> > control impedance. is it ok ?
> > has anyone has other suggestions to the layer
> > stuckup?
> >
> > thanks,
> >
> > Aric Hadav
> > Hardware Design Engineer
> > [email protected]
> >
> > **** To unsubscribe from si-list or si-list-digest:
> > send e-mail to
> > [email protected]. In the BODY of message
> > put: UNSUBSCRIBE
> > si-list or UNSUBSCRIBE si-list-digest, for more
> > help, put HELP.
> > si-list archives are accessible at
> > http://www.qsl.net/wb6tpu
> > ****
> >
>
> __________________________________________________
> Do You Yahoo!?
> Yahoo! Shopping - Thousands of Stores. Millions of Products.
> http://shopping.yahoo.com/
>
> **** To unsubscribe from si-list or si-list-digest: send e-mail to
> [email protected]. In the BODY of message put: UNSUBSCRIBE
> si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
> si-list archives are accessible at http://www.qsl.net/wb6tpu
> ****
**** To unsubscribe from si-list or si-list-digest: send e-mail to
[email protected]. In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu
****
**** To unsubscribe from si-list or si-list-digest: send e-mail to
[email protected]. In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu
****
This archive was generated by hypermail 2b29 : Tue May 08 2001 - 14:30:25 PDT