Do the trace length need to be the same in high speed bus?

[Jos Brink]

routing 25mhz multidrop bus

I'm connecting 2 chips usig a MII bus. Because the bus is high speed (25Mhz), do the trace lenghts of these lines need to be exactly the same length?

Here's a screenshot. is this a good aproach for creating the same length?
it's only a draft, don't mind the litte errors, component text, offgrid placement ect.

layer stack:

green = top
dark grey 3V3
light grey GND
red = bottom

 

[skywalker]

length match 50ps

Hi Jos Brink,

The critical lenght are the total lenght of a single net. Is the lenght of path will connect all pins of the signal.

If the signal source start of center board, and the receivers are one sx and one dx to source, the same lenght of traces are better off course, but the total lenght must be respected.

If the probelm are the various lenght of the signal bus, you need to match with accordion (serpentine traces) all signal bus, but you need a specific h-sped tool for this.

Hope this help, let me know, Skywalker.

 

[sigint]

Re: track length

Having a tool that will do it for you is nice, but it can be done by hand, I was matching lengths to +/- 50 Ps. delay - years before the option was available in other tools.

SiGiNT

 

[Jos Brink]

Re: track length

Thnx alot for helping me out.

what do you mean with "to +/- 50 Ps. delay "?

I'm using ultiboard and you can see the total length of a trace while you are drawing it. but on a 25Mhz bus, how critical is it that they match?

Thnx

 

[skywalker]

Re: track length

Hi, if i'm not in error +/- 50Ps are plus or minus 50 Picosecond, intended for rise time.

For a critical lenght, are not so simple. You need impedance, capacitance, delay (for a correct rise time), and others for correct lenght calculation. With Designer assistance, you can read a data sheet for devices requirements.

Another important argument is the devices used, 25Mhz is not very higher frequency, but using very fast devices, this make a problem.

Best, SKywalker.

 

[jdhar]

track length

It's not important for MII - that doesn't mean route them any length you want, but I have routed MII on a 2-layer board with relatively loose length matching (within 200 mils), and it worked without problems. Match them as best as you can, but it's not 'critical'.

 

[sigint]

Re: track length

Actually the number I cited above is incorrect - I was refering to propagation delay which for FR4 is about 176 pico seconds per inch for internal traces and about 155 pico seconds per inch for external signals - this is a measure of how long it takes a signal to travel a given distance and is determined entirely by the Dielectric Constant of the material the PCB is constructed of, I checked my old files and the job I was thinking of was +/- .025 inch which would equal about +/- 5 pico seconds, this is only a factor when it is important that a signal arrives with precise timing in relation to other signals - you'll frequently encounter constraints of this type when working with differential pairs.

SiGiNT

 

[cyberrat]

track length

So if we have a data bus that is rnning at 25mhz, we have to match the lengths of the nets so that they are all the same?

Funnily enough I'm doing a 25mhz bus this week too, is this the length of the entire net or from point to point (uP to IC)?

 

[jdhar]

track length

You should "try" to match the lengths, but like I said, it's not critical for 25M. And you want the total length to match - if you have a multi-drop bus, each segment shoudl be the same length. If you have point to point, you only need to match the one length.