F-antenna board height

[kbu]

I am placing a F-Antenna on a FR4 board and had a few questions :

- Why does the F-antenna need to be on 2 sides even though an antenna switch is used (e.g. NCB/SRB board)

- what height should I use for the board, i don't have a NCB board with me but I was hoping for a 0.062 inch board (any idea if dielectric properties of FR4 at 0.062 inches will be okay with the F-Antenna?)

- what's the minimum clearance (left and right) I should keep with the antenna?

I've seen the compact antenna's data sheet but it doesn't seem to explain these points.

[bigmac]

Hello,

To which data sheet do you refer?

If you are using a Tx\Rx switch, I cannot see any particular advantage for the antenna to be printed on both sides.  Are the two sides joined using vias?  The board thickness should not be critical.

With some implementations, the Tx antenna was on one side, and the Rx on the other.  In such cases, there would be less interaction between the two sides the thicker the board material.  Even for these cases, I would suspect that 0.062 thickness would be OK (since availability of thicker material would be limited).

The F-antenna is really intended to be located at the end of the PCB,  and not surrounded by other components (or ground plane).  If other components must infringe, the "earthy" end of the antenna should be less critical than the "floating" end.  Application note AN2731 may give some indication of the minimum clearance.

Regards,

Mac

[kbu]

I was referring to AN2731.
So it seems from the gerbers that on the NCB/SRB boards that both sides of the F-Antenna are connected with a via, so basically its the same antenna? (but why then is it on both sides? isn't one side enough considering the circuit uses a switch)

What the appnote AN2731 doesn't specify is the clearance to left and right of the F-Antenna. (bigmac: If the 'earth' end can have some components near by would there be a 'mininum' keep out zone I should consider?)

Also about the thickness of the board the reason I'm worried is that for a microstrip line a lot depends on the dielectric constant of the board, so a 0.031 board will be different than a 0.062 board, so I'm not really sure how much it would throw off the calculations the designers would have used.
Any way, alternatively can someone let me know what the thickness of the NCB/SRB board is (I don't have a dev kit of those boards)

Message Edited by kbu on 2007-03-2803:10 PM

[bigmac]

Hello,

---

kbu wrote:

So it seems from the gerbers that on the NCB/SRB boards that both sides of the F-Antenna are connected with a via, so basically its the same antenna? (but why then is it on both sides? isn't one side enough considering the circuit uses a switch)

---

I would have thought so - but then I don't know what the designer had in the back of their mind.  I might also have expected the two sides to be "stitched" together with many vias.  It is possible that the double sided approach may give a marginally wider operating bandwith.

---

What the appnote AN2731 doesn't specify is the clearance to left and right of the F-Antenna. (bigmac: If the 'earth' end can have some components near by would there be a 'mininum' keep out zone I should consider?)

---

As I indicated in my previous post, the antenna should ideally be totally clear of any obstruction along three edges, and have a ground plane along the fourth edge.  For the ground plane to be effective, I would suspect that the minimum width of circuit board should be about 45 mm.

If you have a much wider board, the antenna might be located in a corner of the board, with no obstruction along two of the edges.  In this case, I would guess that the "earthy" end should probably not have any obstruction closer than about 10 mm.  If obstructions are too close to the antenna, this is likely to reduce the antenna gain, and will affect the omnidirectionality of the radiation pattern.

---

Also about the thickness of the board the reason I'm worried is that for a microstrip line a lot depends on the dielectric constant of the board, so a 0.031 board will be different than a 0.062 board, so I'm not really sure how much it would throw off the calculations the designers would have used.
Any way, alternatively can someone let me know what the thickness of the NCB/SRB board is (I don't have a dev kit of those boards)

---

Yes, the characteristic impedance of any microstrip would be affected, and may need to have track width adjusted to compensate..  Are microstrip sections used for antenna matching purposes?

Regards,

Mac

Message Edited by bigmac on 2007-03-3004:14 AM

[strikecity]

I have successfully copied the SRB reference design with very good results. My advice tips are as follows:
1)Spend A LOT of time reviewing the provided gerbers. I followed Freescale's gerber files within 1 mil for all traces and relative trace positioning. By doing this, my antenna performed as advertised on my first try.

2) No, you don't want to use a 0.062" PCB thickness. To do this, you'd have to make a 115 mil wide microstrip trace between C144 and the F antenna (on the SRB design). The original SRB board was 1mm thick (.0393") because it was specified in Europe. I have it on very good authority (and verified in my design) that if you copy the SRB design onto a 2 layer 0.032" PCB, you need a microstrip width of 56 mils.

3) As other responders have already stated, you should have zero components, traces, etc. on three sides of the antenna, and should have the strongest ground plane possible on the fourth side. Notice that the SRB reference design has ground planes on the top and bottom layers of the PCB. To further enhance the ground plane, they've installed vias along the edge of the ground plane which is parallel to the antenna. My ground plane is identical in width to the SRB plane (~2" wide) and it is 1" deep. If I revise this board, I will probably seek to increase the depth of the ground plane.

4) I got away with a 2 layer PCB. If you look at the SRB design, you'll see that they used 4 layers, but really the two internals weren't exploited heavily. So, if you want to do a 2 layer, it should work fine.

5) Finally, regarding your "why is the F antenna on both sides, I say, "who cares?" I'm just thrilled that I was able to produce a working RF PCB on the first try without going back to school for a master's degree. Follow the reference design, and don't look back.

[Nabla69]

Hi Strikecity,

That is a fantastic report, thank you very much for reporting your experience !

Alphonso.

[joerg]

Hi
if this helps:
the thickness of the MC1321x reference board is 0.94mm (37mil) maybe 1mm (39mil).

Saluti Joerg

[kbu]

Ups.. I mean board thickness!!! (sorry brain freeze)