Replace trace impedance with resistor?

[FriedMule]

I have fount out that a 50 Ohm impedance trace on a PCB is a hard (and expensive) thing to do when we talk about 0Hz-1GHz. Is it possible to use a SMD 50 Ohm resistor instead?

[tszaboo]

Sure. You can also replace an antenna with a 50 ohm resistor, it looks perfect on the VNA. And a coax cable can also be replaced with just a resistor on one end and then regular cable. I dont even know why people spend so much time designing these things, it is so simple.

[FriedMule]

Sure. You can also replace an antenna with a 50 ohm resistor, it looks perfect on the VNA. And a coax cable can also be replaced with just a resistor on one end and then regular cable. I dont even know why people spend so much time designing these things, it is so simple.

Be aware that this is the beginner's section. Your sarcasm may lead the OP to the wrong direction.

Yes and sarcasm is hard to read from his text, not much to hint sarcasm from:-)

[FriedMule]

Maybe I should refrace my question, is there any way to cut down on the price (cheap PCB producer) or a way to at least sort of "guarantee" that I hit 50 Ohms impedance in first try?

I have tried to use https://www.eeweb.com/tools/microstrip-impedance to calculate the impedance
Expect to use a Rogers type PCB

[magic]

Even if you build a proper transmission line, it needs to be terminated with 50Ω to ground at the receiving end anyway, unless the load has built-in termination or it's some external RF connector.

Supposedly you may get away with wrong line impedance if the distance is some 10x shorter than the wavelength. But wavelength at 1GHz is merely 20~30cm so that doesn't buy you much. Even is such case, make it a proper transmission line, with a nice ground return conductor running in parallel at uniform distance.

[Dave]

50 ohm traces are going to be extremely wide on a 2-layer 1.6mm board, but you can simply bump it up to a 4-layer PCB. The latter are not that expensive anymore.

I don't think you need to use special substrates like Rogers, unless your application requires really tightly controlled impedances, which I doubt, considering the question. Regular FR4 is going to be just fine up to a gig.

[Zero999]

To answer the original question: no a 50R trace is not a resistor, but a transmission line with a characteristic impedance of 50R. Look up transmission lines and characteristic impedance.

[FriedMule]

To answer the original question: no a 50R trace is not a resistor, but a transmission line with a characteristic impedance of 50R. Look up transmission lines and characteristic impedance.

Thanks I'll definitely look that up! :-)

Even if you build a proper transmission line, it needs to be terminated with 50Ω to ground at the receiving end anyway, unless the load has built-in termination or it's some external RF connector.

Supposedly you may get away with wrong line impedance if the distance is some 10x shorter than the wavelength. But wavelength at 1GHz is merely 20~30cm so that doesn't buy you much. Even is such case, make it a proper transmission line, with a nice ground return conductor running in parallel at uniform distance.

The probe gets connected to an oscilloscope in that end where the 50 Ohm trace is going to.
LOL 30cm / 10, no that does not give a whole lot to work with:-)

50 ohm traces are going to be extremely wide on a 2-layer 1.6mm board, but you can simply bump it up to a 4-layer PCB. The latter are not that expensive anymore.

I don't think you need to use special substrates like Rogers, unless your application requires really tightly controlled impedances, which I doubt, considering the question. Regular FR4 is going to be just fine up to a gig.

Yes I have read about the 4 layer sollution before but did not understand it at all, could you please explain how 4 layer helps and please on how to layer it? :-)

[Illusionist]

Instead of a 4-layer, you could use double sided 0.8mm board instead of 1.6mm. That's what I did on my GPS board. The reason (for  both options) is that the impedance depends on the thickness of the dielectric between the copper layers.

I do wish people would stop saying how cheap 4 layer boards are... my GPS PCB cost about £3 in two layer. It would have cost more like £43 in 4 layer from JLC, by the time I'm stung for tax and fees on top of the already 10x higher cost.

[Dave]

Yes I have read about the 4 layer sollution before but did not understand it at all, could you please explain how 4 layer helps and please on how to layer it? :-)

With 4 layer boards, you can have a ground plane much closer to the layer you're routing your 50R trace on. The thicker the dielectric between the trace and ground plane, the wider the trace needs to be to meet the impedance.
You would need a 3mm wide trace on a 1.6mm double sided board to meet 50R, while you can use 0.35mm on a 4-layer board with 0.2mm substrate under the outer layers.

4 layer boards also have the added benefit of giving you two extra layers to route other signals under the controlled impedance traces.

I do wish people would stop saying how cheap 4 layer boards are... my GPS PCB cost about £3 in two layer. It would have cost more like £43 in 4 layer from JLC, by the time I'm stung for tax and fees on top of the already 10x higher cost.

I don't know the specifics of your circuit board, but JLC seem to have decent prices on smaller 4-layer boards.
50x50mm @ 10 pieces for 13 USD
100x100mm @ 10 pieces for 29 USD

To me it seems quite cheap these days, considering the fact that they used to be 60-80 USD for 100x100mm @ 10 pieces several years ago.

[Illusionist]

@Dave, I know, and I wasn't really intending to have a go at you.

The trouble is, that $29 PCB is over our 'free' import limit of £15. It will get hit with tax and, worse, £10 to £15 ransom handling fee from the courier. So that $29 PCB lands here at £40+. And it does start out at 10x the cost of the two layer so I still don't think it's that cheap although it is certainly more affordable than it used to be.

A few people have asked JLCPCB to investigate adding the tax at their end. It's possible to do, and then we wouldn't have to pay the additional handling fee here. Just the tax.

Anyway, sorry for the thread drift FriedMule, now back to your regular scheduled programme

[FriedMule]

Dave and Illusionist thanks for your great posts, I have visited the https://pcbshopper.com/ site where you can get prices from several places at once and it looks to me like the difference from 2 to 4 layer is about 3-4 times the price, while the thickness does not really matter.
The solution with using 0.8 instead of 1.6 sounds great but do make the board thinner, is that why some recommends a 4 x 0.4 layer board instead of a 2 x 0.4 layer, to make them less flimsy?

My 4 boards has to be mounted on the side (4.7" x 1.5" - / - 120mm x 39mm) with the same spacing as standard BNC's on a scope is mounted (is there a standard spacing, what is it?) I do not think that 0.8 thickness is a problem here?

The trace design uses Coplanar Waveguide, track width 1.27 mm, gap width 0.2 mm. I do not know the Dielectric Thickness or constant but is that posible just to add in the notes as something like "Please select a FR4 board where a coplanar waveguide, track width 1.27 mm, gap width 0.2 mm gives a 50 Ohm impedance +/- 1 Ohm"?

By the way, I have found a graph, showing losses when comparing a FR4 and a Rogers PCB. Am I right in that thay are nearly the same for an <1GHz 2 1/4 inch (57 mm) trace on a probe board?

[ArthurDent]

Have you considered using a semi-rigid subminiature 50 ohm coax instead of a line built into the board? it would make the board simpler and cheaper. RG405 is only .086' outside diameter and there is also some that is .047" in diameter. Cut to length, form, and solder the ends of the shield to the ground plane on the board. Neat and simple. 

[FriedMule]

Have you considered using a semi-rigid subminiature 50 ohm coax instead of a line built into the board? it would make the board simpler and cheaper. RG405 is only .086' outside diameter and there is also some that is .047" in diameter. Cut to length, form, and solder the ends of the shield to the ground plane on the board. Neat and simple.

Sounds interesting, I am planning to solder some RG400 directly to the end of that 50 Ohm trace but yes totally replacing the trace with a coax sounds logical.
The original designer did say that the 50 Ohm was important, and I think he sis solder some coax to the board after the track, makes me wonder why.

[Illusionist]

0.8mm thickness is indeed flimsier. Whether it's a problem depends on how it will be treated. The problem is that much flexing is likely to crack solder joints of course, and possibly crack MLCC capacitors which tends to have very unfortunate results.

If the PCBs are fixed into the enclosure such that flexing cannot occur, as mine are, then there's no problem. If that can't be done then 0.8mm is a poor idea and you'll need 1.6mm. In that case, if you can't make the traces wide enough on 2-layer to get down to 50Ω, then the above solution of using some thin coax is a workable one.

[FriedMule]

0.8mm thickness is indeed flimsier. Whether it's a problem depends on how it will be treated. The problem is that much flexing is likely to crack solder joints of course, and possibly crack MLCC capacitors which tends to have very unfortunate results.

If the PCBs are fixed into the enclosure such that flexing cannot occur, as mine are, then there's no problem. If that can't be done then 0.8mm is a poor idea and you'll need 1.6mm. In that case, if you can't make the traces wide enough on 2-layer to get down to 50Ω, then the above solution of using some thin coax is a workable one.

I do really like your answer:-) So a thick 2 layer board is the best for stability but useless for impedance of 50 Ohm.
I have made a drawing of what I think I understand, top is how it is now, bottom is your suggestion.
 

[Illusionist]

Well it's ArthurDent's suggestion, but I agree with it. Yes, your diagram has the gist of it.

Whether it's better for your design than a 2.88mm wide trace (which is what you need to get 50Ω on a 1.6mm thick 2-layer board)... only you can tell. I had too much going on close by to put such a wide trace in.

I might end up using the coax method on my next PCB because, other than the impedance requirement on multiple tracks, I have no need to go to four layers. It's too big a board and will have a lot of PCB-mount sockets to risk 0.8mm thickness with. I still need to think about the best way to deal with it.

[FriedMule]

Well it's ArthurDent's suggestion, but I agree with it. Yes, your diagram has the gist of it.

Whether it's better for your design than a 2.88mm wide trace (which is what you need to get 50Ω on a 1.6mm thick 2-layer board)... only you can tell. I had too much going on close by to put such a wide trace in.

I might end up using the coax method on my next PCB because, other than the impedance requirement on multiple tracks, I have no need to go to four layers. It's too big a board and will have a lot of PCB-mount sockets to risk 0.8mm thickness with. I still need to think about the best way to deal with it.

Great, so again I can choose between coax, wider track or flimsy board. Since I am thinking of building some sort of shielding around the board, it may be enough to protect the board?

Is it okay to change the subject in this thread? I mean that I hope to build more boards, each in its own shielding enclosure to shield 0Hz-1Ghz. Each fairly close together. Each board has a BNC female plug and I would like to space the boards such that the BNC plugs has a standard spacing in the front panel.
Questions:
Is there any standard BNC spacing on oscilloscopes?
What material should I use to make the enclosure of?