• State Resolved
  • Locked Locked
  • Replies 9 replies
  • Subscribers 57 subscribers
  • Views 2664 views
  • Users 0 members are here
Support feedback
Options
Options
Related

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

PCB Antenna Impedance Matching - CC253x

InnoPlay
Prodigy 130 points
Other Parts Discussed in Thread: CC2531, CC2541

I have look at many reference designs for your PCB antennas. While I'd like to copy as close as possible, I generally find that I need to move the uC a little farther away or I need to flip the antenna. In either case I find myself computing the trace width to keep a 50ohm impedence match (may not even be saying this correctly). What I have never really understood is where that begins and ends. For instance, looking at the CC2531 USB dongle design, the trace is wide all the way to the balum. I see many designs from other vendors where traces between the device that make up the matching network are as small as 4mil. Are the trace widths in this area critical? Assuming no balum, where do the trace widths matter? My assumption has always been that the traces from the uC to the first devices were thin and from there I would make them as near as possible to the computed value using impedance matching software.

Cheers

  • 0
    TI__Genius 9705 points

    Hi,

    RF trace width is calculated to maintain constant 50Ohm impedance. Based on the stack up of the board, the trace width needed to achieve 50Ohm impedance will vary. It is very important to have a constant impedance trace to avoid mismatch and hence power loss on RF traces. Also, if the footprint for the component on the RF trace is much different from the trace width, it creates impedance discontinuity with the same end result. The components are placed close to each other with constant width trace connecting the components to mimimize impedance discontinuity. Most antenna and equipment used for RF measurements need to see 50Ohm impedance for maximum power transfer. Hence, it is critical to maintain 50Ohm impedance on the trace from the end of matching network to the antenna. It would be best if you can maintain 50Ohm impedance all along from the RF pins to antenna.

    Regards,

  • 0 in reply to SVS
    Prodigy 130 points
    Thanks for the quick reply. Just what I was looking for to understand some of the layouts I've been looking at. Regards
  • 0 in reply to InnoPlay
    TI__Guru**** 317180 points

    Note that a trace that is shorter than about 1/10 of the wavelength will not behave as a transmission line. This is normally the case from the RF_P/ RF_N pins and to the end on the balun/ filter. In this section the trace widths in the ref design is most often a standard width set up in the layout tool. If the trace from the end of the balun towards the antenna is long, a 50 ohm track should be calculated here.

  • 0 in reply to TER
    Prodigy 130 points

    One other note I was curious about. Primarily becuase I have gone through the exercise of measuring the reference design trace widths and designs files and tried to get that information to match up to impedance calculators (and it doesn't)....so in many of TI designs that don't use the balum, the 50Ohm feed point is at the end of the matching network and the antenna is connected at that point so a 50Ohm trace path to the uC is not necessary from the standpoint of trace width but is probably good practice if the width is not 1.3mm.. I assume the matching network provides the required impendance from th euC to the end of the matching network??? There is a 2530 reference design that is very similar to the 2540 keyfob design with the exact same layout but one has thinner traces from the end of the matching network (and feedpoint) back to the uC so that sort of answers that question I suppode.

    Final questions I promise...

    When TI makes the statement about copying the reference design as close as possible, Is the layout of the matching network more critical than board thickness? assuming the PCB trace antenna is connected to the feedpoint that is right at the end of the matching network (like the reference designs I mentioned above)

    The thought here is that a different layout can make the board shorter at the expense of changing the layout of the matching network.

    Is there any advantage of a matching newtwork over one of the balums you use in your designs. That murata balum is pretty small and low cost (cant remember which design you use it in but I have copied that design as well).?

    Thanks All

     

  • 0 in reply to InnoPlay
    TI__Guru**** 317180 points

    Board thickness is more important to some extent at least. The reason for this is the parasitics to ground. If the board thickness change the parasitics change and it could be that the component values have to be changed.

    With a integrated balun you will loose a few dB in link budget but save space and get a simpler design/ layout. Check out the app notes on the topic for CC253x and CC254x to see the difference between integrated and discrete balun.

  • 0 in reply to SVS
    Prodigy 140 points

    Hi SVS

    Could you please check out page 5 of this document http://www.ti.com/lit/an/swra297b/swra297b.pdf. The track width of the transmission line keeps increasing in 3 steps. How does one calculate the impedance of such a line.

    Also if I am unable to place the balun symmetrically with respect to CC2541, can I draw a differential pair from CC2541 RF pins to balun? What can be the maximum track length and width to maintain an impedance of 50 ohm?

    Thanks in advance

    Regards

    Himanshu

  • 0 in reply to Himanshu Jain
    TI__Genius 9705 points

    Hello Himanshu, 

    Reason for increasing width of transmission line in steps is to make the impedance transition gradual rather than an abrupt jump that can cause reflections. The impedance of this trace is the impedance of longest part of the trace.

    The design mentioned in your comment is a 2 layer board. 50 Ohm traces are wider (and often impractical) on 2 layer boards with the stackup used, as can be calculated using a transmission line calculator. However, as TER mentioned, when the trace length is shorter than 1/10 the wavelength of the signal, they need not be considered as transmission lines and the width (impedance) is not critical. However, it is important to keep the traces as short as possible between balun and RF pins. It is highly recommended to place the balun symmetrically wrt CC2541. 

    Regards

  • 0 in reply to SVS
    Prodigy 140 points
    Yes, even our calculations for a 2 layer board gave a very wide track (w/h>1) and, I guess, the general formulae do not apply then. We can keep the RF pins to Balun short but how do we calculate the length and width of the track from the Balun to the External Antenna?

    FR4 material with dielectric constant 4.6
    h = 0.8mm
    t=0.035mm

    We have tried to copy the CC2541 based Postage Stamp design but I am unable to understand the TI calculations for length and width of the trace from the Balun to the Antenna. Also how does the 0ohm resistance affect the calculations? (reference: tidc156a)
  • 0 in reply to Himanshu Jain
    TI__Guru**** 317180 points
    If you have a transmission line you can calculate the width with one of the online calculators listed in this thread: e2e.ti.com/.../1372043