[Arm-netbook] eoma68 rk3288 testing

[Luke Kenneth Casson Leighton]

http://rhombus-tech.net/rock_chips/rk3288/news/

i now have 2 assembled PCBs with the exact same "fault" - which after
talking to paulk and akaka on #linux-rockchip i *may* have a lead on
how to get the DDR3 RAM up and running properly. we believe it's down
to the impedance control register (ZQCR) which is being hard-coded in
u-boot-rockchip rather than being allowed to "train". those values
are suited for 6-layer 1.6mm PCBs - the impedance of tracks when you
have an 8-layer 1.2mm PCB are *half* what they are for 6-layer 1.6mm
PCBs.

l.

---
crowd-funded eco-conscious hardware: https://www.crowdsupply.com/eoma68

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attac

[Hrvoje Lasic]

impedance is function of width of line (with some adjustment of copper
thickness) plus thickness of prepag directly below surface where your lines
are. So, you need to compare what is on your last pcb and what is on your
new pcb. best software to calculate this value is polaris and you can get
some days for free if you ask for code but there are free alternatives out
there like Saturn that we use. Beside that there are differential lines
that you also need to match impedance. I am not sure but I doubt that via
registers you can fix this problem.

also, in some cases you can put resistors in series of lines where you
think you have problem.

basically, you need to find out what impedance need to be and where are you
now in order to fix this, of course if this is really problem.

Post by Luke Kenneth Casson Leighton
http://rhombus-tech.net/rock_chips/rk3288/news/
i now have 2 assembled PCBs with the exact same "fault" - which after
talking to paulk and akaka on #linux-rockchip i *may* have a lead on
how to get the DDR3 RAM up and running properly. we believe it's down
to the impedance control register (ZQCR) which is being hard-coded in
u-boot-rockchip rather than being allowed to "train". those values
are suited for 6-layer 1.6mm PCBs - the impedance of tracks when you
have an 8-layer 1.2mm PCB are *half* what they are for 6-layer 1.6mm
PCBs.
l.
---
crowd-funded eco-conscious hardware: https://www.crowdsupply.com/eoma68
_______________________________________________
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook

[Luke Kenneth Casson Leighton]

---
crowd-funded eco-conscious hardware: https://www.crowdsupply.com/eoma68

Post by Hrvoje Lasic
impedance is function of width of line (with some adjustment of copper
thickness) plus thickness of prepag directly below surface where your lines
are. So, you need to compare what is on your last pcb and what is on your
new pcb. best software to calculate this value is polaris and you can get
some days for free if you ask for code but there are free alternatives out
there like Saturn that we use. Beside that there are differential lines that
you also need to match impedance. I am not sure but I doubt that via
registers you can fix this problem.

http://linux-sunxi.org/A10_DRAM_Controller_Calibration#Impedance_settings.2C_ODT_and_ZQ_calibration

apparently ZQ config registers do exactly that

Post by Hrvoje Lasic
also, in some cases you can put resistors in series of lines where you think
you have problem.

yyyeah not in this case - there's not enough space between the rk3288
and the ddr3 ram ICs to fit 20 0402 resistors, even if i used 4-packs.
i'd need to completely redo the entire DDR3 layout and that's
something that i know will cost about 4 or 5 revisions (and around
$10k in the process).

Post by Hrvoje Lasic
basically, you need to find out what impedance need to be and where are you
now in order to fix this, of course if this is really problem.

yeah i will be checking the PMIC output voltages with a scope
tomorrow. it's fairly certain that it's impedances - going from 290
to 300mhz really should not make a huge difference but it does.

l.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook

[Hrvoje Lasic]

ok, these are internal resistors that help match impedance automatically.
they are calibrated against reference resistors as they are not very
precise. quite smart. but i still think you need to check impedance of your
lines as i assume this calibration process is good to certain point, if
lines are really bad that it cant help. However, you should try to enable
this, maybe it will help.

Also,before redesign all board, check what impedance should be for all
lines (datasheets), go through simulation software what impedance is now.
Check what was impedance on previous version of PCB that worked (go through
simulation again). So, maybe you can just change thickness of prepag (if
that is possible) that match previous version of PCB (if you have same
design of ddr3/mcu).

Post by Luke Kenneth Casson Leighton
---
crowd-funded eco-conscious hardware: https://www.crowdsupply.com/eoma68

Post by Hrvoje Lasic
impedance is function of width of line (with some adjustment of copper
thickness) plus thickness of prepag directly below surface where your

lines

Post by Hrvoje Lasic
are. So, you need to compare what is on your last pcb and what is on your
new pcb. best software to calculate this value is polaris and you can get
some days for free if you ask for code but there are free alternatives

out

Post by Hrvoje Lasic
there like Saturn that we use. Beside that there are differential lines

that

Post by Hrvoje Lasic
you also need to match impedance. I am not sure but I doubt that via
registers you can fix this problem.

http://linux-sunxi.org/A10_DRAM_Controller_Calibration#
Impedance_settings.2C_ODT_and_ZQ_calibration
apparently ZQ config registers do exactly that

Post by Hrvoje Lasic
also, in some cases you can put resistors in series of lines where you

think

Post by Hrvoje Lasic
you have problem.

yyyeah not in this case - there's not enough space between the rk3288
and the ddr3 ram ICs to fit 20 0402 resistors, even if i used 4-packs.
i'd need to completely redo the entire DDR3 layout and that's
something that i know will cost about 4 or 5 revisions (and around
$10k in the process).

Post by Hrvoje Lasic
basically, you need to find out what impedance need to be and where are

you

Post by Hrvoje Lasic
now in order to fix this, of course if this is really problem.

yeah i will be checking the PMIC output voltages with a scope
tomorrow. it's fairly certain that it's impedances - going from 290
to 300mhz really should not make a huge difference but it does.
l.
_______________________________________________
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook

[Luke Kenneth Casson Leighton]

---
crowd-funded eco-conscious hardware: https://www.crowdsupply.com/eoma68

Post by Hrvoje Lasic
ok, these are internal resistors that help match impedance automatically.
they are calibrated against reference resistors as they are not very
precise. quite smart. but i still think you need to check impedance of your
lines as i assume this calibration process is good to certain point, if
lines are really bad that it cant help. However, you should try to enable
this, maybe it will help.

i'll find out tomorrow soon enough. current settings are hard-coded
to 40ohm driving and 155ohm termination (in the processor dram) which
seems very odd.

Post by Hrvoje Lasic
Also,before redesign all board, check what impedance should be for all lines
(datasheets), go through simulation software what impedance is now. Check
what was impedance on previous version of PCB that worked (go through
simulation again). So, maybe you can just change thickness of prepag (if
that is possible) that match previous version of PCB (if you have same
design of ddr3/mcu).

not a chance. increasing the line thickness to 4mil increases the
impedance by something like 4%. there's no way i can use anything
other than 1.2mm boards. there's ABSOLUTELY no way i can go to 6
layer. and the dielectric constant for 6mil board separation would
have to be reduced to something insane like 1.0 in order to claw back
the reduction in separation.

this *has* to have been taken into account in the design of DDR3
drivers / receivers, that there would be circumstances where the
impedance is off like this.

l.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments

[Hrvoje Lasic]

Post by Luke Kenneth Casson Leighton

Post by Hrvoje Lasic
Also,before redesign all board, check what impedance should be for all

lines

Post by Hrvoje Lasic
(datasheets), go through simulation software what impedance is now. Check
what was impedance on previous version of PCB that worked (go through
simulation again). So, maybe you can just change thickness of prepag (if
that is possible) that match previous version of PCB (if you have same
design of ddr3/mcu).

not a chance. increasing the line thickness to 4mil increases the
impedance by something like 4%. there's no way i can use anything
other than 1.2mm boards. there's ABSOLUTELY no way i can go to 6
layer. and the dielectric constant for 6mil board separation would
have to be reduced to something insane like 1.0 in order to claw back
the reduction in separation.
this *has* to have been taken into account in the design of DDR3
drivers / receivers, that there would be circumstances where the
impedance is off like this.

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. so, if you have for example 4 layer board you
have copper conductor, then substrate then copper conductors etc and all of
this are i.e. 1.2 mm thick. But when you calculate impedance you take into
consideration only layer that is below surface if you line is on top (and
because most signal lines are on top of PCB, if lines are in the middle of
PCB board there are different calculation).

example here (h- thickness of prepreg)

http://chemandy.com/calculators/microstrip-transmission-line-calculator-hartley27.htm

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. You have to tell them you need
12 layer board and my layer of prepreg must be so and so thick, what can
you offer me... Maybe this is possible, maybe not.

[Luke Kenneth Casson Leighton]

Post by Hrvoje Lasic
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.

Post by Hrvoje Lasic
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-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-***@file

[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.

Post by Luke Kenneth Casson Leighton

Post by Hrvoje Lasic
I am not sure if we understand each other here. Impedance of your lines

are

Post by Hrvoje Lasic
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.

Post by Hrvoje Lasic
So, for thickness of your lines you need to match with thickens of

prepreg

Post by Hrvoje Lasic
to be able to meet certain impedance. it does not mean that your total

PCB

Post by Hrvoje Lasic
thickens must be changed, you can vary some other layers of preprag,

there

Post by Hrvoje Lasic
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.
_______________________________________________
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook

[Luke Kenneth Casson Leighton]

after finding various bits of documentation i'm going to be testing
out the following settings, which match the (known, calculated)
impedance of the EOMA68-RK3288 board (around 50-60 ohms instead of
100-120 of the Reference Design):

http://www.skhynix.com/product/filedata/fileDownload.do?seq=6790
MR1: bits 9,6,2 = b001 = RZQ/4 = 60 ohms ODT
bits 4,3 = b00 = CAS disabled
bits 5,1 = b00 = RZQ/6 = 40 ohms output driver impedance
bit 7 = 0 = write-leveling disabled
bit 11 = 0 = TDQS disabled
bit 12 = 0 = output disabling not enabled
bit 10 reserved
bit 8 reserved
MR2: bits 10,9 = b01 = RZQ/4 = 60 ohms ODT
bits 6,5,4 = b001 = CAS Write Latency 6
bits 3,2,1 = b100 = partial array self-refresh 3/4 array

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-***@files.phco