Oscillation in RF Power Amplifier (Avago MGA-412P8)

amplifier oscillation

Dear Friends

I made an RF amplifier using Avago MGA-412P8). The schematic and component values follow description in MGA-412P8 datasheet.

I build the circuit on FR4, with dielectric height of 1.6 mm.

When I measure the RF amplifier with no RF input, I find oscillation in around 1.5 GHz in its harmonics. I have tried to move some components around the RFIC, but the oscillation always occurs.

What the source & cause of the oscillation?

Thank you very much for your help.

Regards,
Fracosoe

rf design avoid self oscilation

Hi,

some points,

Hope you have Land pattern as per recommendation and have soldered the center ground tab to ground .
While measuring connect termination at the input with a load or attenuator.Dont leave it open.

Use good quality inductors(with high self resonance frequency) like those from Coilcraft.

regards
GV

power amplifier oscillation

When you made the PCB from 1.6mm FR4, the circuit is effectively very different from original application cause you have around 2.5mm width 50 ohm traces. An additional series inductance is created at the input/output ports. Also the vias have much higher inductance compared to original design. These conditions are likely to cause oscillations.

It may be possible to achieve stable operation on 1.6mm FR4, but it's a different design.

rf amplifier + oscillations

I don't like the FR4 for frequencies below 300 MHz.
Check de dielectric constant of your material.
Decoupling, etc.

After all, did you connect a 50Ω charge for measurement?

Best regards

amplifier oscillation measure

The design is made on 10 mil/0.254 mm thick Rogers RO4350 board (see text below fig 5 in the data sheet). This laminate has an effective er 3.66, to be used for RF design according to Rogers Corp data sheet. The width of the input/output 50 ohm microstrip conductors has a width of 0.55 mm. The input/output matching circuits in the data sheet is designed for matching to 50 ohm.

But if you use the same width (0.55 mm) on an FR4 PCB, having 1.6 mm thickness, the input/output microstrip conductors will have an impedance of about 110 ohms, using an effective er of 4.3 for the FR4. Correct width is 3.1 mm for a 50 ohm microstrip transmission line on FR4 (1.6 mm thick, er of 4.3).

If you now connect the input/output of your FR4 amplifier board to a 50 ohm system, an impedance transformation will take place between the input RF connector at the PCB edge and the RF input of the chip. The 0.55 mm wide transmission line is about 8.6 mm long between these two points. The chip RF input, which was matched to 50 ohm via L5/L6/C1, will now instead see a different impedance. The attached simulation shows it will see about 79 +j61 ohms at 2.45 GHz, which is a return loss of about 6.5 dB. A similar mismatch will take place at the RF output of the chip. These mismatches may very well cause instability of the amplifier.

There is also a short transmission line TL1 (width 0.56 mm) in the circuit diagram, its impedance will also be changed when FR4 is used.

oscillation causes

hi

1.desing the PCB as per the reference design and pour the copper on bottom and top side of the PCB and add gnd vias as much as possible arround the RF path(since u are using FR4, but he is using FR4 with copper ROGER R04350).
2. measure the impedance at the i/p and o/p port, if this is not near to 50 ohm you need to fine tune by using the i/p and o/p matching elements.
[/code]

rf amplifier oscillation

For some reasons MGA-412P8 is a very unstable PA, even if you follow the AVAGO PCB specifications. Especially the bias lines (pin 4 and 6) need critical decoupling and careful ground design.

rf amplifier oscillation problem

vfone said:

For some reasons MGA-412P8 is a very unstable PA, even if you follow the AVAGO PCB specifications. Especially the bias lines (pin 4 and 6) need critical decoupling and careful ground design.

Click to expand...

How do you know that MGA-412P8 is highly unstable?
Please give me guidance for decoupling (capacitor) design or calculation and ground design. Is it the ground at bottom layer or top layer that need careful design?

Thanks.

Added after 51 minutes:

disisku_22 said:

hi

1.desing the PCB as per the reference design and pour the copper on bottom and top side of the PCB and add gnd vias as much as possible arround the RF path(since u are using FR4, but he is using FR4 with copper ROGER R04350).
2. measure the impedance at the i/p and o/p port, if this is not near to 50 ohm you need to fine tune by using the i/p and o/p matching elements.
[/code]

Click to expand...

Please explain the reason of point 1. Why I must place gnd vias as much as possible?
IMHO, it will affect the impedance of RF transmission line (input & output), because the TL changes from microstrip line to stripline or coplanar waveguide.

thanks.

Added after 22 minutes:

GVVIN said:

Hi,

some points,

Hope you have Land pattern as per recommendation and have soldered the center ground tab to ground .
While measuring connect termination at the input with a load or attenuator.Dont leave it open.

Use good quality inductors(with high self resonance frequency) like those from Coilcraft.

regards
GV

Click to expand...

All of inductors used in the RF Amplifier have resonant frequency > 3 GHz, so I think there should be no problem with them.
I have also soldered the ground tab below the RFIC to ground. However, I cannot make vias with small radius, therefore I place no via below the RFIC. I just connect the ground below the RFIC with two vias outside the RFIC footprint.

My PCB design is attached.

Secondly, do leaving input termination open cause permanent damage?
The oscillation and its harmonics still exist after I connect the input port to signal generator.

Thanks.

rf power amplifier grounding substrate

I think that VSWR is right. You need to have your proto done exactly as vendor recommended. Their engineers know their own ICs better than anybody here. Pay attention to the parts types: they must be exactly as vendor recommended. Replacing any parts with the same value but another vendor often lead to different circuit behavior due to different RF properties and/or parasitic. Even via diameter and spacing must be the same as recommended. Do not put upper ground plane if vendor did not put it.

Here is a couple of tricks how to deal with oscillation when it exists despite all your efforts. You may connect an open stub to the output and adjust its length to the oscillation frequency. Practically you make it longer and then cut by small pieces and adjust. You may use semiflexible or semiridgit 47mils or 86 mils coaxial cables or printed stubs. If you cut it check possible DC shortage before cut or disconnect power supply, which is better. This is very effective for prototyping. Next point: if your prototype is in the box try to remove the cover. If oscillation goes away when you remove the cover it is cavity oscillation and you need to make the smallest size of the box smaller. Sometimes absorber can be put inside the box, but most of the times you need to redesign the box or use internal partitions.

Best regards,
RF-OM

avago ads power amplifier

The PCB design confirms the doubts voiced by VSWR and me regarding consequences of using 1.6mm FR4. You have those rather long trace segments with > 50 impedance.

However, I cannot make vias with small radius, therefore I place no via below the RFIC. I just connect the ground below the RFIC with two vias outside the RFIC footprint.

Click to expand...

The worst thing however (I already feared somthing like this) is the ground connection of the exposed pad. I can't imagine, that the amplifier can become stable without changing it. My general opinion is, you can probably use FR4 (with higher losses, of course). A lot of economic 2.4GHz circuits is using it. But you can't use a 1.6mm board and you need smaller vias for a suitable ground connection.

tl mga-412p8

I’ve tried to integrate MGA-412P8 into a multi-standard wireless card and I got these problems. This PA has some internal design issues, most probably a lack of minimum internal decoupling capacitors or other internal layout issues, making in this way the chip very sensitive chousing the external ground and placing the external components.
If you have time can try to evaluate other PAs from different manufacturers (the market is full of options).

If you want somehow to avoid the long vias parasitic inductance try to use a solid top layer ground plane, as much as you can.

mga power amp

I just want to say couple words about FR4. The major problem with this material is not the losses, but not stable Er. It is hard to get good repeatability of board performance with FR4. I used this material up to 6GHz and it may work well when controlled impedance is not so important. Via may be optimized even for 1.6 mm substrate especially for not so high frequency as 2.4GHz. By the way, today there are other materials on the market that outperform FR4, work well up to 10GHz and cost about he same as FR4. I used one of them and everything was okay even for printed high Q bandpass filters in 3-5 GHz range.

BR,
RF-OM

50 ohms lead on fr4 width?

RF-OM said:

I just want to say couple words about FR4. The major problem with this material is not the losses, but not stable Er. It is hard to get good repeatability of board performance with FR4. I used this material up to 6GHz and it may work well when controlled impedance is not so important. Via may be optimized even for 1.6 mm substrate especially for not so high frequency as 2.4GHz. By the way, today there are other materials on the market that outperform FR4, work well up to 10GHz and cost about he same as FR4. I used one of them and everything was okay even for printed high Q bandpass filters in 3-5 GHz range.

BR,
RF-OM

Click to expand...

I used FR4 after reading that so many papers using FR4 for antenna. I thought if it's good for antenna, it must be good also for circuit at 2.4 GHz.

Btw, Please inform me the new material that outperform FR4.

Thanks.

rf power amplifier vendor

The limited Er stability of FR4 (I noticed, that a wide range of Er is allowed according to IPC standard, partly narrowed by manufacturers) isn't a particular issue for wideband applications.

But you won't improve stability with a RF substrate if not reducing parasitic inductances.

fr4 pcb working 5ghz range

Rogers RO4350, RO4000 etc are excellent replacements. See comparison between RO4000 and FR4 here:

http://www.rogerscorporation.com/mwu/techtip4.htm

Fig II in this article shows the result of er 4.2 ±0.2 variation (bandpass filter as an example). My experience from FR4 is more worse: er can vary from 3.8 to 4.6 from batch to batch, from manufacturer to manufacturer and over temperature.

Btw, Please inform me the new material that outperform FR4.

Click to expand...

rf amplifier 2.4 ghz circuits

Rogers have very good materials but they are expensive. There is Nelco 4000-13 with stable up to 10GHz Er=3.7 and very low variations from lot to lot. The loss tan=0.008 and price is very close to FR4.

I disagree that for very wide band applications Er is not important. When board substrate has wrong Er all traces will have wrong impedance which in turn will exaggerate reactance multiplying effect of the traces. This is actually not parasitic but rather transmission line intrinsic property. Filters based on printed structures will be completely destroyed if Er change more than certain limit. Wide band RF and microwave applications usually required so called controlled impedance boards when vendor control manufacturing process in order to keep characteristic impedance of the lines in required limits.

Best regards,
RF-OM

rf amplifier oscillations

There's nothing I like to contradict. RF substrates have a obvious advantages. I just wanted to emphasize two points:
- A lot of economic RF designs is using FR4.
- The issue giving the title of this thread doesn't come from using FR4

bias oscillation power amplifier

Dear FvM,

I agree that FR4 is good as inexpensive material. For about a year I switched to Nelco because it has the same price but demonstrate excellent repeatability of board's parameters that you cannot achieve with FR4. Even sensitive interdigital band pass filters are repeatable with Nelco. There are also some materials from GE that are modifications of FR4, but we decided that Nelo is better. We even use it for UWB antennas. I definitely can recommend this material for controlled impedance RF and microwave boards up to 10 GHz. Did not check it for higher than 10 GHz frequencies yet, so cannot tell how good it may be above 10 GHz.

Best regards,

RF-OM

rf pa unstable at low frequencies

vfone said:

I’ve tried to integrate MGA-412P8 into a multi-standard wireless card and I got these problems. This PA has some internal design issues, most probably a lack of minimum internal decoupling capacitors or other internal layout issues, making in this way the chip very sensitive chousing the external ground and placing the external components.
If you have time can try to evaluate other PAs from different manufacturers (the market is full of options).

If you want somehow to avoid the long vias parasitic inductance try to use a solid top layer ground plane, as much as you can.

Click to expand...

vfone...
Did you continue to use MGA-412P8 or you change to other PA?
If you continue, how to make the MGA work?

I have connect 1000pF to pin 4. It reduces the harmonics significantly, but not affecting the fundamental of oscillation.

Please recommend good PA for me to be operated on WLAN a/b/g.

Thanks

power amplifier oscillation

I never used MGA-412P8 in production and I choused a PA from a different manufacturer. There are plenty of other choices on the market for this application (RFMD, SiGe, Anadigics, Skyworks). Just go to their websites and ask for a quotation and samples.