Hey. I read a long long time ago about how 486 motherboards couldn't go past 33MHz front size buss because a lot of the traces had right angles. And there were these new special motherboards which could run at 40MHz FSB because they had 45 degree angles or less only.
My understanding is that any hard angles in a PCB trace would cause RFI and probably reflections. Between leakage and smearing, it apparently can effectively destroy the signal. Is this basically correct? Does anyone know exactly what a hard angle does to the signal from a transmission line perspective? Would it maybe look like ESR and/or ESL?
So wouldn't it be best to have nice soft curves instead of hard angles in the traces? I seems logical to me. Do any digital PCB guys use curved traces in practice? Do any of the PCB fabrication houses someone like a DIYer might use support them?
Lastly, I am curious what if any effect curved traces might have on audio bandwidth analog signals? I am guessing virtually none.
My understanding is that any hard angles in a PCB trace would cause RFI and probably reflections. Between leakage and smearing, it apparently can effectively destroy the signal. Is this basically correct? Does anyone know exactly what a hard angle does to the signal from a transmission line perspective? Would it maybe look like ESR and/or ESL?
So wouldn't it be best to have nice soft curves instead of hard angles in the traces? I seems logical to me. Do any digital PCB guys use curved traces in practice? Do any of the PCB fabrication houses someone like a DIYer might use support them?
Lastly, I am curious what if any effect curved traces might have on audio bandwidth analog signals? I am guessing virtually none.
Hi Cameron,
90° angles in PCB traces won't work with fast edges, as you correctly state. The right-angle represents an impedance change in the line, because the conductor is wider at a right angle, and therefore the parasitic capacitance is higher. A right angle in a transmission line behaves like a gate attached to the transmission line at the same point.
If for whatever reason you need the line to bend 90° at a point, don't worry, there's an easy workaround. You can either radius the outside of the bend, to keep the conductor width constant, or chamfer the outside at a 45° angle to 57% of the line width. Either way will maintain good impedance control. Using two 45° angles close together is probably easier.
If you look at a fast PC motherboard you can see curved traces, mostly in delay lines. Some PCB layout programs can generate these curves and other can't. Similarly, only some prototype PCB manufacturers are capable of producing them.
For digital audio, where you will normally be working at speeds of < 50MHz and rise times > 5ns, the rule of thumb is to always use 45° angles in traces. Beyond that, there are more important improvements you can make, none of which involve curved traces.
90° angles in PCB traces won't work with fast edges, as you correctly state. The right-angle represents an impedance change in the line, because the conductor is wider at a right angle, and therefore the parasitic capacitance is higher. A right angle in a transmission line behaves like a gate attached to the transmission line at the same point.
If for whatever reason you need the line to bend 90° at a point, don't worry, there's an easy workaround. You can either radius the outside of the bend, to keep the conductor width constant, or chamfer the outside at a 45° angle to 57% of the line width. Either way will maintain good impedance control. Using two 45° angles close together is probably easier.
If you look at a fast PC motherboard you can see curved traces, mostly in delay lines. Some PCB layout programs can generate these curves and other can't. Similarly, only some prototype PCB manufacturers are capable of producing them.
For digital audio, where you will normally be working at speeds of < 50MHz and rise times > 5ns, the rule of thumb is to always use 45° angles in traces. Beyond that, there are more important improvements you can make, none of which involve curved traces.
Curved Traces
I use PADS 3.5.1 to design PCBs and I use curved corners all the time on my traces. At an EMI class I was told they are less prone to radiate and they are no big deal to use. If you can't do this, then, always miter the corners with 2 45°angles instead of a single 90° bend. And any story about some motherboards having 90° angles would maybe have applied to one manufacturer with a stupid board layout person singe mitering the corners with 2 45° bends has been common practice singe the very first PC boards.
I use PADS 3.5.1 to design PCBs and I use curved corners all the time on my traces. At an EMI class I was told they are less prone to radiate and they are no big deal to use. If you can't do this, then, always miter the corners with 2 45°angles instead of a single 90° bend. And any story about some motherboards having 90° angles would maybe have applied to one manufacturer with a stupid board layout person singe mitering the corners with 2 45° bends has been common practice singe the very first PC boards.
Re: Curved Traces
This is a myth:
http://www.signalintegrity.com/Pubs\edn\bigbadbend.htm
dmfraser said:
This is a myth:
http://www.signalintegrity.com/Pubs\edn\bigbadbend.htm
Corners
So they have no effect according to the link posted. Nice to hear another legend destroyed. However, mitered corners, whether radiused or done with dual 45° bends look prettier. At least I think so.
But then I think some village in Texas is missing its Harvard educated idiot and others disagree with me about that too as is their right.
So they have no effect according to the link posted. Nice to hear another legend destroyed. However, mitered corners, whether radiused or done with dual 45° bends look prettier. At least I think so.
But then I think some village in Texas is missing its Harvard educated idiot and others disagree with me about that too as is their right.
Re: Re: Curved Traces
That seems like a weird rebuttal, because on the very same guy (Howard Johnson) advises against 90° corners in his book High-Speed Digital Design. I'd also propose that most DIY designs don't use 8-mil microstrip no FR-4. You're much more likely to be working at 20-mil or larger.
Mainly i think 90° bends look bad!
tiroth said:
That seems like a weird rebuttal, because on the very same guy (Howard Johnson) advises against 90° corners in his book High-Speed Digital Design. I'd also propose that most DIY designs don't use 8-mil microstrip no FR-4. You're much more likely to be working at 20-mil or larger.
Mainly i think 90° bends look bad!
PCB Houses
I have dealt with 2 PCB houses and had no complaints about curved traces. The Gerber files that PADS 3.5.1 generates do not seem particularly larger when there are curves.
And, if nothing else, 90° curves do indeed look bad. I know no one cares about the looks of the PCB but if I can make it look good for little more effort, why not.
---------------------------------------------------------------
A wise man changes his mind when presented with new evidence. A fool stays the course no matter what.
I have dealt with 2 PCB houses and had no complaints about curved traces. The Gerber files that PADS 3.5.1 generates do not seem particularly larger when there are curves.
And, if nothing else, 90° curves do indeed look bad. I know no one cares about the looks of the PCB but if I can make it look good for little more effort, why not.
---------------------------------------------------------------
A wise man changes his mind when presented with new evidence. A fool stays the course no matter what.
I'm new at this and have a couple of questions.
1) From what has been said in the post about resistance and such, traces should be uniform in width for the entire trace, but does this include ground lines? Or can you make the ground lines bigger and odd shapes to fill open space?
2) What exactly is a grounding plane and what is it's purpose?
3) For T shaped traces, should the trace be made to look like a Y, with all 45° angles, or can you make one trace straight, with a single branch breaking off in 45° angle. (Hope this makes sense)
Any help would be appreciated.
1) From what has been said in the post about resistance and such, traces should be uniform in width for the entire trace, but does this include ground lines? Or can you make the ground lines bigger and odd shapes to fill open space?
2) What exactly is a grounding plane and what is it's purpose?
3) For T shaped traces, should the trace be made to look like a Y, with all 45° angles, or can you make one trace straight, with a single branch breaking off in 45° angle. (Hope this makes sense)
Any help would be appreciated.
queens49 said:
I assume we're talking about digital. Impedance should be uniform on a transmission line. If the line is so short that it doesn't need to be modelled as a transmission line, then just do whatever you want. For anything long enough to matter, the impedance needs to be constant and the line needs to be terminated. Normally you want the trace width and the height above the ground plane to be constant.
A digital signal should be thought of as a loop. For any current travelling from A to B, there is a current travelling from B to A. The ideal path for this current (on a printed circuit board) is directly under the trace. The ground plane provides this return path.
Avoid t-shaped traces. If you have to bifurcate a trace, make it Y-shaped. However, please note that if you make a Y-shaped trace, you must make each leg of the Y double the characterstic impedance of the stem. If you have more than two loads, just put them evenly spaced along the same transmission line and terminate it at the end, or use a quad driver to drive them all point-to-point.
I must say this has turned out to be an awesome thread! I guess I will go with curved traces because: It seems most pcb fabs support it. There is no particular reason not. And it just looks cool. 
On the topic of ground planes and current loops, how does the power supply and local bypass caps fit into that picture? In a few analog only designs, all my caps are rail to rail. I am wondering if I need a connection to ground with a little current flow, what does that current loop look like? I am also wondering if by not having rail to ground caps near this, I am creating a current loop which goes all the way back to the power supply, which in this case is not terribly close.
On the topic of ground planes and current loops, how does the power supply and local bypass caps fit into that picture? In a few analog only designs, all my caps are rail to rail. I am wondering if I need a connection to ground with a little current flow, what does that current loop look like? I am also wondering if by not having rail to ground caps near this, I am creating a current loop which goes all the way back to the power supply, which in this case is not terribly close.
Thanks for the information JWB.
Just to clarify the answer to the grounding plane question. For digital signals, you basically require 2 traces. One considered the signal trace, and the other is the "return" trace, that is on the grounding plane. In other words, 2 traces from Point A to Point B than?
I'm not sure if you are familiar with MWP's DAC-3 implementation, but on his PCB artwork, he has lots of copper fill areas, that I'm guessing is connected to ground. Would the purpose of this is to help reduce interference from outside sources?
Just to clarify the answer to the grounding plane question. For digital signals, you basically require 2 traces. One considered the signal trace, and the other is the "return" trace, that is on the grounding plane. In other words, 2 traces from Point A to Point B than?
I'm not sure if you are familiar with MWP's DAC-3 implementation, but on his PCB artwork, he has lots of copper fill areas, that I'm guessing is connected to ground. Would the purpose of this is to help reduce interference from outside sources?
There are two reasons for power planes.
1st is to keep the impedance of the power supply small reducing effects like ground bouncing and over shots.
2nd is that the field of each signals traces closes to the power (ground) plane what gives a constant impedance and less cross talk.
Regards
130nm
1st is to keep the impedance of the power supply small reducing effects like ground bouncing and over shots.
2nd is that the field of each signals traces closes to the power (ground) plane what gives a constant impedance and less cross talk.
Regards
130nm
One of the main reasons for early PC circuit boards hitting the wall with increased clock freq, was that even the separate lines of the buses had different routes and lengths along the PCB, probably as a result of uncritical use and lousy quality of early autorouters.
Talking characteristic impedance on a FR4 substrate is a rather duboius business, because of of production spread in the substrate itself. The general rule of transmission lines is that if your conductor is longer than 1/10 th of the wavelength, general transmission theory should be applied,- i.e. should be regarded as a transmission line. Assuming a velocity factor of appx. 0,5, your trace limit is 15 cm for 100 MHz. This of course only applies to double sided or multilayer boards, as you need a plane or mirror conductor to form the distributed capacitance for a transmission line.
The general rule for PCB layout used to be that below 100 MHZ, you could more or less get away with anything , impedancewise.
From roughly 100 MHZ to apppx 1GHz, caution had to be applied, and above 1G was black magic. This is still partly true, as stray capacitance and serial inductance can play some nasty tricks , unless you know what you are doing. Still it is amazing what you can get away with, - just have a look inside some satellite TV tuners.....
For digital signalling in time critical designs, it is common practice to route buses parallell, with equal length, but even more important is termination resistance. The latter probably has more influence on the waveform than the actual PCB trace.
As for Queens asking about the ground plane....
Particularly for RF work, it has been common practice to use double sided PCBs, where one side, usually top side, is used to make all ground connections. This have several advantages, - it gives better control of stray capacitance, as it refers most of the stray to ground, - the plane. It will also somewhat simplify the layout, as it places all ground connections on one side, - but is also adds capacitance in the circuit, as all traces on the routing side now form a small capacitance to ground plane.
There is as such no problems in using the same technique in audio boards, - double sided with one plane as ground, but again, - it increases capacitance somewhat,- an absolute no-no to some designers. The technique of filling voids on a PCB with planes. ground connected or not, is usually called a "cooper pour" in modern PCB software. Tha plane can be solid, hatched, etc. but more important, - at some PCB plants you pay pr. etched square inch, - thus it can also be an econimical issue. A modern multilayer board is usually produced in reverse, - you deposit copper electrolytically on a basically bare fiberglass plate.
As for the rounded traces and corners, it is an old gospel that sharp corners should be avoided, aslo among RF engineers. For audio, I seem to recall reports of some "Golden Ears" clearly hearing the difference!
In sum , I think we all agree to the thesis of short traces, whether they be curved or angled, - and it doesn't hurt if it looks nice, - does it??? As for production of boards with curved traces, - if the PCB house does not have "your" software, which they probably don't, - they will be using your Gerber files, - with your self made curves..( read: your own curves.... )
No problem.
Talking characteristic impedance on a FR4 substrate is a rather duboius business, because of of production spread in the substrate itself. The general rule of transmission lines is that if your conductor is longer than 1/10 th of the wavelength, general transmission theory should be applied,- i.e. should be regarded as a transmission line. Assuming a velocity factor of appx. 0,5, your trace limit is 15 cm for 100 MHz. This of course only applies to double sided or multilayer boards, as you need a plane or mirror conductor to form the distributed capacitance for a transmission line.
The general rule for PCB layout used to be that below 100 MHZ, you could more or less get away with anything , impedancewise.
From roughly 100 MHZ to apppx 1GHz, caution had to be applied, and above 1G was black magic. This is still partly true, as stray capacitance and serial inductance can play some nasty tricks , unless you know what you are doing. Still it is amazing what you can get away with, - just have a look inside some satellite TV tuners.....
For digital signalling in time critical designs, it is common practice to route buses parallell, with equal length, but even more important is termination resistance. The latter probably has more influence on the waveform than the actual PCB trace.
As for Queens asking about the ground plane....
Particularly for RF work, it has been common practice to use double sided PCBs, where one side, usually top side, is used to make all ground connections. This have several advantages, - it gives better control of stray capacitance, as it refers most of the stray to ground, - the plane. It will also somewhat simplify the layout, as it places all ground connections on one side, - but is also adds capacitance in the circuit, as all traces on the routing side now form a small capacitance to ground plane.
There is as such no problems in using the same technique in audio boards, - double sided with one plane as ground, but again, - it increases capacitance somewhat,- an absolute no-no to some designers. The technique of filling voids on a PCB with planes. ground connected or not, is usually called a "cooper pour" in modern PCB software. Tha plane can be solid, hatched, etc. but more important, - at some PCB plants you pay pr. etched square inch, - thus it can also be an econimical issue. A modern multilayer board is usually produced in reverse, - you deposit copper electrolytically on a basically bare fiberglass plate.
As for the rounded traces and corners, it is an old gospel that sharp corners should be avoided, aslo among RF engineers. For audio, I seem to recall reports of some "Golden Ears" clearly hearing the difference!
In sum , I think we all agree to the thesis of short traces, whether they be curved or angled, - and it doesn't hurt if it looks nice, - does it??? As for production of boards with curved traces, - if the PCB house does not have "your" software, which they probably don't, - they will be using your Gerber files, - with your self made curves..( read: your own curves....
)No problem.
You are absolutely right with analogue signals. Even to use the top layer as ground plane instead of using multi layer gives you more than twice the distance of the build capacitor reducing it to less than half the capacity.
I came from high speed digital design and thought the thread was about this. In this case multi layer is a must! Imagine you have 64 data lines switching simultaneously at less than a nano second with a drive strength of more than 100mA peak each. You simply cannot put this on a two layer board including ground plane because your traces take too much space. AMD made the socket 939 to enable board designers to get to 4 layer boards what wasn't possible with socket 940 which required six layer boards.
Differently routed signals on the data bus are a killer. I saw a 50MHz design fail because of some nano seconds lost.
Regards
130nm
I came from high speed digital design and thought the thread was about this. In this case multi layer is a must! Imagine you have 64 data lines switching simultaneously at less than a nano second with a drive strength of more than 100mA peak each. You simply cannot put this on a two layer board including ground plane because your traces take too much space. AMD made the socket 939 to enable board designers to get to 4 layer boards what wasn't possible with socket 940 which required six layer boards.
Differently routed signals on the data bus are a killer. I saw a 50MHz design fail because of some nano seconds lost.
Regards
130nm
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.