FEDEVEL
Platform forum

SARBAZ13 , 08-04-2016, 02:55 PM

HI ROBERT
HELP ME - ROUTING SDRAM FOR LPC1788
LAYER: 2LAYER(TOP-BOTTOM)
SDRAM: K4S561632H-UI75
I'M ROUTING ADDRESS-DATA-COMMAND
IS LENGTH MATCHING IT RIGHT?
THANK'S ROBERTS

SARBAZ13 , 08-05-2016, 12:16 AM

HI
HELP ME ROBERT

mairomaster , 08-05-2016, 01:50 AM

The length matching seems fine to me, from what I can see in the first screenshot, although not all signals are visible. A tip here is to enable the signal length column (right click on the column titles). Currently you only have routed length, which is not that accurate all the time.

You might want to leave slightly more space between the separate tracks and between the waves in a single track if possible, to reduce crosstalk.

SARBAZ13 , 08-05-2016, 11:16 AM

HI MAIROMASTER
How much space should be between track?
width track: 0.2mm
clearance : 0.2 mm
layer : 2layer
mcu: lpc1788 FBD208

SARBAZ13 , 08-05-2016, 11:48 AM

width track: 0.2mm
clearance : 0.2 mm
layer : 2layer
mcu: lpc1788 FBD208

is it true figure under for spacing between track?

mairomaster , 08-05-2016, 02:10 PM

Have you taken the Advanced PCB Layout course? Those things are explained very well there. If you haven't, here you can learn about the particular topic:



0.2 mm clearance seem alright for manufacturing purposes. However, I was speaking about cross talk between the tracks. Because of that it is good to leave a bit more space between high-speed tracks. 3 times the track width is a generally safe value. Also it's good to have a bit wider waves, because of self cross talk withing a signal. Just watch the youtube video, everything is explained there

robertferanec , 08-07-2016, 04:30 AM

@SARBAZ13 I am not 100% sure about length matching on 2 layer PCB. Even you length match the signals correctly, the power distribution to the chips and crosstalk between the tracks may cause a lot of problems and it may not work reliably. Maybe in your case the length matching may cause more problems than benefits.

Try to find reference designs and have a look how others did that. I do not have eagle installed, but maybe this could help you: https://www.olimex.com/Products/Modu...ource-hardware

SARBAZ13 , 08-07-2016, 02:37 PM

hi robert
CAN you convert eagle to ALTIUM AND SEE(REFERENCE VIDEO ALTIUM)
I SEE YOUR LINK.BUT IT'S 4LAYER
QUESTION:
1-IS SIGNAL ADDRESS & DATA & COMMANDS LENGTH MATCHING?(OLIMEX BORAD PCB NOT LENGTH MATCHING.WHY?)
2-I DESIGNE 4 LAYER BORAD IS BETTER?
3-IS IT DESIGNE 2 LAYER BAD?


THANKS REGARDS

robertferanec , 08-08-2016, 02:22 AM

1) It may not be required. The memory is probably slow and the tolerance for length matching may be bigger, so the routed tracks may be in tolerance even they do not use the "waves" to adjust the length.
2) yes
3) yes

To understand points 2) and 3) from crosstalk point of view, use a crosstalk calculator (e.g. https://www.eeweb.com/toolbox/microstrip-crosstalk/ ) and play with it. Use values which you have used in your design (the distance between tracks, stackup, ...) and compare the results (Cross Talk Coefficient, Coupled Voltage) between 2 layer PCB and 4 layer PCB. You will see how bad two layer is ... plus, your real results will be much worse as you do not have solid reference plane under your tracks. Also, there are some other disadvantages of two layer PCBs ....

SARBAZ13 , 08-10-2016, 12:39 PM

hi robert
QUESTION:

2-Whether to 4 layers have a total thickness range is 1.6 mm?
L1(0.4) + L2(0.4) + L3(0.4) + L4(0.4) = 1.6MM

SARBAZ13 , 08-11-2016, 01:28 PM

Where are you, Mr. Roberts.

mairomaster , 08-11-2016, 03:21 PM

Can you clarify the question, please?

1.6 mm is a standard thickness of a low class 4 level PCB. For a high-speed PCB you normally use either thinner PCB or higher layer count. One of the reasons for that is to decrease the separation between signal layers and ground reference planes, which improves your signal integrity (cross-talk etc.).

Normally you don't have equal thickness for all layers. You would have less space between L1-L2 and L3-L4 for example. That again helps for the signal integrity with a thicker, 4 layer board. Then you can have (L1, L4) signal layers and (L2, L3) reference ground/power layers for example.

SARBAZ13 , 08-12-2016, 11:09 PM

hi mairomaster
thickness board :0.5mm
thickness copper:18um
L1:36um L2:18um L3:18um L4:36um
What should be the core value?
What should be the prepeg value?

robertferanec , 08-13-2016, 12:16 AM

@SARBAZ13 these are very specific PCB manufacturing questions and the best place to ask is your PCB manufacturer as they know what kind of material they have and they can suggest a stackup which is possible to manufacture.Plus, consider the notes from @mairomaster

SARBAZ13 , 08-22-2016, 11:29 PM

HI ROBERTFERANCE

I have sdram to part number K4S561632H-UI75
how to simulation sdram by altium?

mairomaster , 08-23-2016, 01:44 AM

Take a look here:


I would rather not bother with simulating in Altium though. From what I've heard from many people, its not really good. And with SI simulations even a very good software can't help you many times.

robertferanec , 08-23-2016, 08:53 AM

@SARBAZ13 your question looks so simple "How to simulation sdram by altium", but it's not easy to answer. Simulation itself is quite a big topic and simulation of memories can be difficult and not easy to explain. Because you have SDRAM, the simplest thing what you can try is to simulate pin to pin connection and check reflections possibly crosstalk. For this, you will need to add models of the components into your library and generate a pulse to see what will happen on the track. For more information you may want to google for "altium simulate" and read the documentation or watch the videos.

I do not use Altium for simulation (if needed I use Hyperlynx owned by some of my clients). I found Altium simulator giving not expected results in some situations (e.g. when I was playing with shape of tracks).