0
\$\begingroup\$

I have doubt how to length matching (if necessary, idk if it is really necessary). Iam checking a layout board in my company and looking on it I realized theres a mismatch for RS-485 communication using chip MAX485E.

I have a connector which I will read MODBUS using RS-485 protocol and looking on MAX485E datasheet it states that differential driver output R= 27ohm (RS-485).

I think it means I need to do length matching for this impedance, but how to calculate it using Saturn calculator, for instance or any other calculator like Kicad calculator?

I would like to know how to calculate trace width and gap to route differential pair in this situation. I have a 2 layers board, using FR-4 (Er=4.6) ; TanD = 0.02 ; Height of substrate (thickness): 1.6mm ; Rhou = 1.72e-08. Im using Kicad with diff pair width = 0.2mm and width gap = 0.25mm set as default in Software. If someone have any document to help me about theory too gonna be good.

enter image description here

\$\endgroup\$
4
  • \$\begingroup\$ Don't worry, this is not ethernet or wifi. \$\endgroup\$ Jun 4 '19 at 20:44
  • \$\begingroup\$ How fast does your RS485 run? \$\endgroup\$
    – Voltage Spike
    Jun 4 '19 at 21:46
  • \$\begingroup\$ State your interface design specs clearly. Cable type, length impedance, bit rate number of nodes. The MAX485E could function with a load from 10 ohms to 320 Ohms and a 3nS rise time. Doesn't mean you have to. What do you have? need? \$\endgroup\$ Jun 4 '19 at 23:12
  • \$\begingroup\$ Did you want 16kV ESD immunity? outdoor lightning immunity too? Is cable TBD or already installed? You have to know all the requirements before you start a design. The IC Tx is actually closer to 20 ~23 Ohms single ended typ. Is it HDX or FDX? ( 2 terminators or 1 ) Is this just for one MODBUS app? Trace Length matching and trace impedance are not your issues if close to the connector. \$\endgroup\$ Jun 4 '19 at 23:57
1
\$\begingroup\$

At the typical feature size of a circuit board, that matters for signals in the GHz. RS-485 isn't even close to that fast.

\$\endgroup\$
6
  • 1
    \$\begingroup\$ Transmission line effects typically start at ~50MHz \$\endgroup\$
    – Voltage Spike
    Jun 4 '19 at 21:48
  • \$\begingroup\$ @laptop2d Show me an RS485 line which runs at ~50MHz =P \$\endgroup\$
    – DerStrom8
    Jun 6 '19 at 0:27
  • \$\begingroup\$ @DerStrom8 Thats exactly my point, some people do run them at 100Mbps \$\endgroup\$
    – Voltage Spike
    Jun 6 '19 at 0:48
  • \$\begingroup\$ @laptop2d The ANSI/TIA/EIA-485 standard only covers up to 10% of that (10Mbps) if I remember correctly. \$\endgroup\$
    – DerStrom8
    Jun 6 '19 at 1:18
  • \$\begingroup\$ @DerStrom8 There are some companies that make non standard transceivers to run at higher speeds \$\endgroup\$
    – Voltage Spike
    Jun 6 '19 at 4:29
1
\$\begingroup\$

RS485 uses differential signaling for the cable of 100Ω or 120Ω, the terminating resistance should match the cable. While it is not necessary or a requirement to match the PCB 'stubs' it's probably a good idea if the speeds of your RS485 bus are high (+50MHz). If they aren't that high, then don't worry about matching on the PCB, but use the correct terminating resistors and cables.

High-speed bus nodes require the application of controlled impedance transmission lines to assure low electromagnetic interference (EMI). On the bus side, the differential impedance of the bus traces must match the characteristic impedance of the transmission medium (100Ω or 120Ω). On the control side, the line impedance of the single-ended traces is commonly set to 50Ω.

Controlled impedance lines are accomplished through well-defined trace geometries (length, width, height, and trace spacing) and close electrical coupling with a low-inductance reference plane, either ground or power. This is easily accomplished with a bus node consisting of a transceiver and controller. However, if you add lightning protection components, such as the surge resistors and transient suppressors shown in Figure 13, the design quickly becomes more complicated.

In this case, the spacing of the differential traces is widened, which causes the differential impedance to deviate from its intended value. This constitutes an impedance discontinuity causing reflections and EMI. While discontinuities might be unavoidable, they should be lumped together to keep their area small.

Figure 13:

enter image description here Source: https://www.renesas.com/us/en/www/doc/whitepapers/interface/high-speed-rs-485-data-links.pdf

If you are using matching then as Renasas suggests, use 50Ω from the microprocessor or FPGA to the tranciever and match the differential pair to the stub (100Ω or 120Ω)

This is the screen for differential pairs (I haven't filled in all the numbers), Make sure you select FR-4 (Er=4.6) and the correct height for your PCB. The width and spacing can vary, the height is determined by your PCB:

enter image description here

This is for a microstrip line, you can choose the width to get the right impedance, Make sure you select FR-4 (Er=4.6) and the correct height for your PCB

enter image description here

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.