[Arm-netbook] eoma68 rk3288 testing

[Hrvoje Lasic]

OK, understood, quite a lot of constraints. anyway, for calculation of
individual traces impedance you can use satrun pcb software. it is free and
has number of other calculation that are nice.

https://www.saturnpcb.com/pcb_toolkit.htm

At the time we made our PCB we also checked impedance with PCB producer
(they make you strip of the board you use with same lines you have on your
PCB and they physically measure impedance). It was quite close match to
what we calculate with Saturn software). Hope it helps.



On Tue, Mar 7, 2017 at 8:52 PM, Luke Kenneth Casson Leighton <lkcl at lkcl.net>
wrote:

> On Tue, Mar 7, 2017 at 7:22 PM, Hrvoje Lasic <lasich at gmail.com> wrote:
>
> > I am not sure if we understand each other here. Impedance of your lines
> are
> > not function of thickness of board and thickness of line but thickness of
> > prepreg and thickens of line.
>
>  understood (and not expressed clearly before that i understand).  so
> please adjust prior reading to understand that i was talking about the
> distance between each of the 8 layers being reduced to 6mil (on a
> 1.2mm stack) where they were, in the Reference Design, well over 10mil
> (on a 1.6mm stack).
>
>  PADS has an unusual feature in that you can specify the stack
> entirely, including distance between layers, thickness of copper
> between layers, dielectric constant of each prepreg and also the
> dielectric constant and thickness of coatings top and bottom.
>
>  from that - and the thickness of tracks - PADS can calculate an
> advisory figure for impedance for each pin-pair or net.  it can't do
> invdividual traces unfortunately.
>
>  i've been using this feature to do investigations, it matches well
> with the capability of the javascript-based calculator you kindly
> posted.
>
>
> > So, for thickness of your lines you need to match with thickens of
> prepreg
> > to be able to meet certain impedance. it does not mean that your total
> PCB
> > thickens must be changed, you can vary some other layers of preprag,
> there
> > are number of options with producers of PCB.
>
>  the amount by which the prepreg of the required layers (1, 3 and
> 8)would have to be changed  is so great as to *require* the total PCB
> thickness to also be changed.  that cannot happen because then the
> case would not fit: there is a hard limit of 4.8mm.  1.2mm is for the
> PCB, 1.9mm for TOP components, and 1.6mm for BOTTOM.  it's therefore
> simply *not possible* to go beyond a 1.2mm PCB thickness.  the
> micro-sd card would need to be removed, for a start, a new type of
> PCMCIA connector sourced (due to the altered height).... i don't
> believe the processor would even fit.
>
>  also, increasing the thickness of the lines to beyond 4mil is also
> not possible, because this is a 0.6mm pitch BGA and there simply isn't
> room to get the lines out from between 2 BGAs (it's already only
> clearance of 3.5mil).
>
>  there *really is* no way to even *begin* to look at doing anything
> *remotely* like a redesign, as the design constraints are so strict
> and so complete that what i have is *literally* the only option.
>
>  yes i tried with 6 layer only but the routing of micro-sd, LCD, eMMC
> and GPIO was so horrendous that it was just far too risky to
> contemplate (as in: almost certain to fail).  as it was, it was six
> weeks before i was happy to even put $1.5k towards the (resultant)
> 8-layer board.
>
>  anyway.  i'll be back at my host's house later today, so can test out
> ZQ auto-calibration, see what happens.  must rest.
>
> l.
>
> _______________________________________________
> arm-netbook mailing list arm-netbook at lists.phcomp.co.uk
> http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
> Send large attachments to arm-netbook at files.phcomp.co.uk
>
-------------- next part --------------
An HTML attachment was scrubbed...
URL: <http://lists.phcomp.co.uk/pipermail/arm-netbook/attachments/20170307/f4510db1/attachment.html>