| Electronics > Projects, Designs, and Technical Stuff |
| Differential active RF probe design queries |
| << < (2/2) |
| dzseki:
Probably not that relevant but I would just remove all thermals from the ground vias, they have no purpose other than increasing the grounding impedance... |
| Nitrousoxide:
--- Quote from: dzseki on December 05, 2018, 09:34:23 am ---Probably not that relevant but I would just remove all thermals from the ground vias, they have no purpose other than increasing the grounding impedance... --- End quote --- Good spot, thank you very much. |
| pigrew:
I'd probably route the power along the edge of the board, in order to keep the bottom ground pristine under the RF elements. Perhaps remove the GND under the SMA pin on the top, so the pin doesn't short to the ground accidentally. What is the block of metal on the bottom under the input connectors? Shouldn't it be grounded? Do you need a series 50-ohm resistor (or pair of 100 in parallel) on the output to set the output impedance? A schematic would help. What is the shunt component on the output? ESD protection diode? I doubt that it helps much to have the groups of four GND vias, perhaps distribute them more evenly? Maybe add a spot to add a bit of resistance or a ferrite to the voltage inputs, in order to filter HF? Add a capacitor+resistor on the input to force some particular input impedance??? (Maybe you have this already on the schematic?) Also, perhaps change to a through-hole connector on the input, in order to have better mechanical stability? The layout is so defined by component sizes and not trace widths that I don't think that the trace's impedance will have much of an effect at 1 GHz. Probably down-sizing components could help, but I don't have enough experience to say what size to use at 1 GHz. Round the corners of the board and perhaps add some mounting holes? |
| Nitrousoxide:
--- Quote from: pigrew on December 05, 2018, 08:55:51 pm --- 1. I'd probably route the power along the edge of the board, in order to keep the bottom ground pristine under the RF elements. 2. Perhaps remove the GND under the SMA pin on the top, so the pin doesn't short to the ground accidentally. 3. What is the block of metal on the bottom under the input connectors? Shouldn't it be grounded? 4. Do you need a series 50-ohm resistor (or pair of 100 in parallel) on the output to set the output impedance? A schematic would help. What is the shunt component on the output? ESD protection diode? 5. I doubt that it helps much to have the groups of four GND vias, perhaps distribute them more evenly? Maybe add a spot to add a bit of resistance or a ferrite to the voltage inputs, in order to filter HF? 6. Add a capacitor+resistor on the input to force some particular input impedance??? (Maybe you have this already on the schematic?) 7. Also, perhaps change to a through-hole connector on the input, in order to have better mechanical stability? The layout is so defined by component sizes and not trace widths that I don't think that the trace's impedance will have much of an effect at 1 GHz. Probably down-sizing components could help, but I don't have enough experience to say what size to use at 1 GHz. Round the corners of the board and perhaps add some mounting holes? --- End quote --- I numbered and addressed these in order: 1. Thanks, will route power along edges. 2. Would that really be an issue? I don't see it happening if it is soldered like any other component. Plus, not that it's critical for this frequency. But for much, much higher frequencies would you not need to maintain the coplanar waveguide for the entire transmission line? 3. Yes. it should be. However, I was having issues with peeling back soldermask on Altium. I realised you had to do it in the "Bottom solder" layer. 4. Added series 50 ohm termination. The shunt component was for an optional protection device. 5. Shifted around all the vias to be more uniform (that was my original intent). Attempted to use Altium's automatic via stitching feature. I guess its kinda useful if you're working on large boards. Takes a bit to tweak the numbers right. 6. Yes. Input already has a 10 Meg nominal impedance. One of the potential problems I might have is the distance mismatch between the two paths. (Highlighted in white in the first post) Im not too sure if that would cause any issues. 7. I havent really given mechanical stability much thought. I dont really intend to stress the probe that much. Final thoughts would be to place it in a snap together case and just use a clamp to hold it. Or to simply not stress it too much. I also reshaped the front of the board to remove excess copper. Top: Bottom: |
| dzseki:
I'd wote against ground pour under the input connector pads, as it acts as a considerable (single ended) capacitance to ground. Also you do a favour for yourself if you'd choose a lower input impedance than 10M, because you can be very sure at 1GHz you input impedance will be nowhere near to that, as it will be governed by parasitic capacitances. That wide range of input impedance change can lead to funny (missleading) things during measurements. |
| Navigation |
| Message Index |
| Previous page |