0
\$\begingroup\$

Could you please let me know if my board needs impedance control? I'm designing a camera board using the IMX225LQR image sensor. After drawing schematic I contacted a company for PCB design and sample manufacture. But they asked me if I need an impedance controlled board which makes additional costs of $200~$300. I have no idea if I really this.

The system clock frequency of the image sensor will be between 27~72Mhz. And this camera board would not have any MCUs and RAMs. I would provide the system clock from outside of this board using PWM of STM32F407. The size of this board is 40mm x 50mm which means the line of trace shouldn't be so long.

this is the data sheet of the image sensor - http://www.ryida.com/upfile/IMX225LQR-C_E_TechnicalDatasheet_Rev0.2.pdf

\$\endgroup\$
  • \$\begingroup\$ Related: electronics.stackexchange.com/questions/13955/… \$\endgroup\$ – W5VO Feb 23 '16 at 5:25
  • \$\begingroup\$ What is the electrical interface type, 3.3V CMOS? What matters more than the clock frequency is the edge rate, or rise/fall times of the clock. If that 50MHz clock has a rise time of say 2ns, and we assume a propagation delay of say 150ps/in in FR-4, then using the rule-of-thumb of electrical length / 6, we end up with (VERY rough!) traces that are around 2.2 inches in length, or ~55.9mm needing to be considered as transmission lines. You could also do the microstrip math yourself, fab the board and see what it ends up being. \$\endgroup\$ – Krunal Desai Feb 23 '16 at 6:54
1
\$\begingroup\$

I've had a quick browse through the datasheet and it seems that the highest data frequency can be about 270MHz.

In all likelihood, no, you shouldn't need the extra service. If it was something like USB 3.0 (@5Gbps+), or PCIe (@2.5Gbps+), then it would definitely be worth considering, but 270MHz is borderline between considering things as distributed vs. lumped, especially if the traces are relatively short.

The board will require careful design, that is for sure. Designing the board with impedance matched traces by design (even without the verification step they offer) should still be done, even if it is an approximation. Also, ensuring you observe differential routing requirements correctly is a must (don't start routing the '+' trace down one side of the board and the '-' trace down the other!).

If this is a prototype run, it's almost certainly not worth it in your case - if the prototype does fail you can always revision, though trying to get it right first time is better. If it was a high volume production run, it would be worth the extra as the cost of high volume would basically trump any the extra cost.

From what I understand, the "controlled impedance" option is basically just a case of using a higher spec substrate and them doing tests to ensure it is the required impedance, vs. making the trace a certain width and hoping it is correct. This related question is worth reading regarding that.

| improve this answer | |
\$\endgroup\$
0
\$\begingroup\$

Probably it will work fine, but.

  1. Any digital signal, even your clock, contains harmonies upt hundreds of megahertz and more (unless it looks like a sine wave), so controlled impedance will reduce risk of radiated emissions, which would first hurt your image.
  2. Impedance control of pcb itself is not enough, digital signal must also be properly terminated.
  3. I have never heard from suck cost for pcb impedance control. Manufacturers calculate it for free, you just define trace width, clearance and stackup. In your case, just define 5 mil on internal layera and 8 mil on external, and let it go.
  4. Don't do it for analog signals. Instead, make their traces wide- 10 or 12 mil. To avoid parasitic inductance.

Upd. Your sensor has digital outputs. Definitely do impedance control.

| improve this answer | |
\$\endgroup\$
  • \$\begingroup\$ (2) termination is closely related to impedance control, actually. (3) is flat-out wrong. You design your board with specific trace widths, dielectric material and thickness, but to guarantee impedance, your manufacturer has to carefully test it and adjust their process accordingly. \$\endgroup\$ – Jay Carlson Feb 23 '16 at 5:37
  • \$\begingroup\$ 2- yes, but aren't we talking about pcb? I was specific about it. 3- i usually decide about that together with manufacturer, when the 2d image is ready. The manufacturers then can adjust dielectric thickness to achieve whatever impedance i require (although there were couple of times that i had to change something for that) \$\endgroup\$ – Gregory Kornblum Feb 23 '16 at 5:42

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.