Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

[SOLVED] Help with operation of phase shifter using SPDT switch

Status
Not open for further replies.
S

sarslanali

Junior Member level 2
Joined
Aug 12, 2011
Messages
24
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,505
I am designing a phase array antenna for my final year project. For phase shifting part I am using skyworks SPDT Switch AS213-92LF. As there is no model available for simulating the switch, so I directly designed and tested the phase shifter. The PCB is shown in the picture. It is not final PCB, as you can see. The problem is that I am getting S11 about -6 db, S22 about -7 and S12 about -10 db, which is very poor performance. Please tell me what can I do to improve performance. I am using 50 ohm line on FR-4 substrate and operating frequency is 2.4 GHz. Please its urgent. PCB.jpg
 

I would taper the lines at the switch, to reduce the discontinuity.
This will also give room to place the ground via near the switch.

64_1343674852.png
 

Thanks for the quick reply. I have few more questions.

1. Does placing the ground via near the switch makes any difference?

2. Where should I short the digital ground with rf ground? The black wire at the two sides are the digital grounds which I have used. Should I short it at the middle pin of rf switch?

3. Should I place the capacitors as near as possible to the rf switch pins? Will it make any difference?
 

place a gnd via as close to the gnd pin of the switch as possible, that will most probably make a difference.
i guess the all bottom layer is gnd. use it as both rf and dc gnd.
desolder the sma connectors, put some gnd vias at the gnd pins of the sma conn, and solder them back. filling the vias with solder wont degrade the performance.
placing some shunt caps like 47-100pF at dc ctrl voltages, as close to chip as possible might also help, and a bigger cap like 1uF at anwhere on pcb.
places of the series dc block caps wont differ much leave them as they are, you may try using smaller ones but not crucial,
and check if your lines are really 50ohm, ie if you are able to print a quick pcb, put only 50 ohm straight line with same lenght on your phase shifter pcb and measure s11 and s21 of the line with same type of sma connectors
good luck
 

kh4n said:
and check if your lines are really 50ohm, ie if you are able to print a quick pcb, put only 50 ohm straight line with same lenght on your phase shifter pcb and measure s11 and s21 of the line with same type of sma connectors
good luck
Click to expand...

Definitely do this. I've used through hole mounted coax connectors as edge launch connectors before (much cheaper that way), but at high frequencies it can cause significant reflections since you're only using two of the ground pins on the connector.

So just make a few test transmission lines, and try it with the line running in different directions to see if that makes a difference (it might on FR4). Then try doing the normal layout, but replace components along different paths with 50ohm strips and see that you still get a good match. Keep building it closer to the final circuit until you find the problem.
 

Thanks for the replies.
I will test the transmission line but as I have said I am building a phased array antenna, so I have already used this line width ( 2.55 mm for FR-4, Er = 4.3) in wilkinson power divider and single inverted-f antenna. I tested them after fabrication and they show good match with simulation in HFSS and have Zo of 50 ohm. Line width for 50 ohm was also simulated in HFSS after initial calculation AppCAD. If you are insisting tomorrow I will again try with transmission line.

1. But is this kind of behavior common with rf ic ? I mean its totally different from what they have shown in data sheet.

2. Do I have to use two DC block capacitors in between switches as I have used in the picture or only one will suffice? These capacitors were given in the data sheet for one switch ( 3 cap for 1 switch). And they said that they are necessary for proper operation of GaAs switch for positive voltage operation. They suggested 100 pF cap for freq>500 MHz.
 

sarslanali said:
1. But is this kind of behavior common with rf ic ? I mean its totally different from what they have shown in data sheet.
Click to expand...

It can be totally different, if the layout is totally different from what the manufacturer uses/recommends. For the switch ground, you have introduced a large series inductance and placed the ground via far away from the switch - big difference, move it much closer. For the "digital" signals, you have used a narrow line of unknown length - possible difference. You can decouple the digital line by using a large series resistors very close to the switch. From what I have seen in the data sheet, the control signal has very little current, so the resistor will pass the control signal and decouple possible RF signals.

For the series capacitor in the RF line, one capacitor is enough. One capacitor blocks DC, so what is the value of adding a second capacitior there?
 

volker_muehlhaus said:
For the "digital" signals, you have used a narrow line of unknown length - possible difference. You can decouple the digital line by using a large series resistors very close to the switch. From what I have seen in the data sheet, the control signal has very little current, so the resistor will pass the control signal and decouple possible RF signals.
Click to expand...

Thanks for the reply. For the digital lines, I will be controlling the lines using microcontroller. I thought that for the digital lines of the rf ic, the line length or width of the line does not make any difference. i think I was wrong. I just wanted to reduce the control lines effort by joining two lines for the switches. So,

1. Should I give separate control signal for each switch?

2. I bought 1000pF 1206 package smd cap for the decoupling. Should I place large series resistor ( as you have said) with these 1000pF to the ground and as close to the pins as possible?

3. In the given PCB, I have used different package 100 pF cap ( As you can see some are large while others are small) will they make any difference?
 

sarslanali said:
1. Should I give separate control signal for each switch?
Click to expand...

I think you can use 4.7kOhm resistor directly at each switch, and connect them to the same digital line.

https://www.skyworksinc.com/uploads/documents/APN2015.pdf
https://www.skyworksinc.com/uploads/documents/200193D.pdf

sarslanali said:
2. I bought 1000pF 1206 package smd cap for the decoupling. Should I place large series resistor ( as you have said) with these 1000pF to the ground and as close to the pins as possible?
Click to expand...

Not sure if it is required, because the 4.7kOhm already provide some isolation from the RF signal.
If you want to add the cap, not sure if 1nF is the best value (-> self resonance frequency?)

sarslanali said:
3. In the given PCB, I have used different package 100 pF cap ( As you can see some are large while others are small) will they make any difference?
Click to expand...

I would check by experiment: put them in the middle of a line and measure S11 & S21.
 

volker_muehlhaus said:
I would taper the lines at the switch, to reduce the discontinuity.
This will also give room to place the ground via near the switch.

64_1343674852.png
Click to expand...

Yeah, those two little thru holes in red in your sketch are VITAL to this switch performance. The line between the thru hole to ground and the ground pin on the switch has to be VERY SHORT! You can still fix it by drilling a tiny hole thru the board at those two places, and soldering a short bus wire from top to bottom. If the distance from switch pin 2 to backside ground is more than 0.100 inch, forgetaboutit!

If it were me, I probably would have chosen a SP2T switch that was an absorptive type, not the reflective type you chose.
 

1. I just wanted to add 1000pF to the control lines because it will be connected to microcontroller and I read at some place that it is added to reduce noise of digital signal.

2. As for the 4.7 kohm resistor, isn't it already available in the switch? Because the resistor is not mentioned in the datasheet anywhere. But the document you mentioned uses 5 kohm with FET.

I bought these switches because only they were available here and I didn't know much about them. May be I did not search enough on internet about them. But I have bought them, so I have to use these switches.

I will also try to drill hole in the PCB tomorrow, if possible
 
Last edited:

You might be ok. Whenevery you put two SP2T switches together with a short line length between them, you run the risk of having a resonance. If you look at the "off" arm, they look like RF short circuits when in isolation mode. So switch 1 is specified as 20 dB isolation, and switch two is also 20 dB isolation, but at one frequency where the line length is N*(1/2 wavelength) you will have a strong resonance, and the combination of the two switches might only yield 15 dB isolation total!

If you have a single frequency where the isolation gets very bad, but is ok far away in frequency, that is probably the problem (assuming you fix the via hole on pin 2, of course). An absorptive switch kills the resonance, and you can have a broadband isolation of 20 + 20 =40 dB.
 

sarslanali said:
2. As for the 4.7 kohm resistor, isn't it already available in the switch?
Click to expand...

I don't know. It only came to my mind as a possible error source, in addition to the ground via placement.

It would be great if they had an application note giving more details.
 

Just one more question:
1. Where should I place the DC block cap between the two switches? Right now they are at the points marked yellow in the picture. Should I replace it with only two cap at the positions marked red in the picture?





Thanks for all your help. I will follow these suggestions and let you know if there is any improvement. Please let me know if there is anything more which I am missing.
 

Attachments

  • pcn.jpg
    pcn.jpg
    1.4 MB · Views: 123
Last edited:

wont matter much, you can leave them at yellow marked places to avoid building a new pcb, but if next pcb version is the case than leave only one at the centre, location wont matter much.
 

Thanks for all your help. I was busy in my project so I could not post the results. I built a new PCB using your suggestions. It worked with satisfying results. I m uploading pictures of pcb as well as measured results. The RF cable I used with VNA machine was not of very good quality. Thanks again for your help. I hope it would help someone in future.

Untitled2.jpgUntitled3.jpg
 

sarslanali said:
I am designing a phase array antenna for my final year project. For phase shifting part I am using skyworks SPDT Switch AS213-92LF. As there is no model available for simulating the switch, so I directly designed and tested the phase shifter. The PCB is shown in the picture. It is not final PCB, as you can see. The problem is that I am getting S11 about -6 db, S22 about -7 and S12 about -10 db, which is very poor performance. Please tell me what can I do to improve performance. I am using 50 ohm line on FR-4 substrate and operating frequency is 2.4 GHz. Please its urgent.View attachment 77936
Click to expand...

You have a problems of dielectric substrate. it not operated at designed of the frequency.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top