Hi VolkerYour layout shows have very few vias. Do you have enough vias to connect top ground with inner ground layer? The eval PCB shown in the data shows the required placements and amount of vias.
Also, can you show a detail photo of your RF connectors at the PCB? Often there is a gap between conector griund and PCB ground, which introduces series inductance.
An important design detail of the original eval board are the vias connecting the exposed pad to the ground plane. Also via fences for the input and output lines.
Original PCB is apparently two layer Rogers, 50 ohm traces are 0.5 mm wide.
View attachment 170220
I agree the vias might have been on the lower end.. but do you think that will reduce its gain to 1dB gain (while it has a gain of 15dB)
Hi Volker,Yes, vias are of extreme importance here. All grounds must be stitched together with small spacing, otherwise the "open end" segements of ground are no longer ground and create unpreditable parasitics.
At the connector, there is no clean transition from SMA ground to effective PCB ground. Just imagine the current path including the (few) vias. At the center pin, I think impedance is much below 50 Ohm: wide pad and small distance to ground.
In addition, there is a gap between coax ground (body) and PCB ground. This will hurt especially at higher frequencies.
I did a quick check of your 50 Ohm line dimensions, that looks ok if vias connect the botoom + side ground properly.
I thought the PCB top layer ground with a via (or two) would be sufficient. You can see the vias in the below figure (forgot to color those for the amplifiers pad). There's not many of them, but they do connect the ground layers to one another. It's just hard for me to understand that adding more vias in the PCB ground for the SMA ground to connect it to the rest of the ground would push the gain by 14dB higher.At the connector, there is no clean transition from SMA ground to effective PCB ground
Is there anything I can do about this? Or verify that this is behind the gain loss?At the center pin, I think impedance is much below 50 Ohm: wide pad and small distance to ground.
There's not many of them, but they do connect the ground layers to one another. It's just hard for me to understand that adding more vias in the PCB ground for the SMA ground to connect it to the rest of the ground would push the gain by 14dB higher.
Thank you FvM. I'll take that into accountAdditional point, you generally don't want thermals for SMD pads on microwave PCB, although they ease hand soldering and rework. You should rather follow the ground connection style used on the evaluation board, particularly for bypass capacitors, additional amplifier ground pads, connectors. Notice that power supply bypass capacitors have lower distance to amp and wider connection trace on eval board.
Hi BigBossYour soldering are too bad and VIAs are very few around GND Connection of the Connectors.This IC has a capability to give typical 25dBm Output Power but the board should have been tested with a VNA first at low RF level. Because if there is no protection circuit, transient regime may blow the IC while testing.SMA Connectors re not very appropriate for 5.8GHz so you should use high quality Touching Type ( short inner PIN ) SMA Connectors.
WR-SMA SMT Edge Card for PCB 1.6mm Max. | Electromechanical Components | Würth Elektronik Product Catalog
Mount End Launch | Connector Type SMA | f DC~18 GHz | Order Samples Free of Charge & Request Quotes Online | High Quality | Fast Deliverywww.we-online.com
Volker that would be great! Maybe even tell me what tools you use to do it, so I can adopt your method in the future.Yes, I saw those vias, but it's far from what an RF designer would create. You have lots of small issues in many places, and these can add up to a large problem.
Regarding the wide pad, you need to control (reduce) shunt capacitance there. One option might be to keep out the inner ground layer and/or increase spacing to side grounds. I usually use EM simulation to design such transitions.
If you want to upload your Gerber file, I can do a quick EM simulation of your existing layout.
Volker that's amazing work! thank you so much. I'll actually learn how to use that EM solver of yoursHi Susan,
I simulated your PCB using my 3D EM solver (Empire XPU). Results show issues with the PCB (poor matching from coax to amp) but total gain is not as bad as you reported. There must be some additional issue.
Circuit simulation is linear simulation (small signal) using the manufacturers S-Params for HMC407.
BR, Volker
You Sir are amazing!!Yes, as I mentioned earlier (before simulations) the transition to coax looks bad: to wide pad = too much shunt C = too low line imepdance.
I did a quick test withtwothree modifications to the input section:
- cutout in ground plane under the pad, to reduce excessive shunt capacitance
- added via fence for proper connection of grounds
- added more vias at the ground pads
With that change, matching of the input section is very much improved already.
PS: Looks professional? I hope so, that's the work that I am doing for the last 25 years as an RF simulation specialist ...
Hi VolkerYes, as I mentioned earlier (before simulations) the transition to coax looks bad: to wide pad = too much shunt C = too low line imepdance.
I did a quick test withtwothree modifications to the input section:
- cutout in ground plane under the pad, to reduce excessive shunt capacitance
- added via fence for proper connection of grounds
- added more vias at the ground pads
With that change, matching of the input section is very much improved already.
PS: Looks professional? I hope so, that's the work that I am doing for the last 25 years as an RF simulation specialist ...
We use cookies and similar technologies for the following purposes:
Do you accept cookies and these technologies?
We use cookies and similar technologies for the following purposes:
Do you accept cookies and these technologies?