Right angle traces

[talvor]

Hi, I currently in the process of laying out my first PCB for an 8x8 RGB LED Matrix.

I would like to know if using right angle traces is a bad thing? And if so why.

Thanks
Phillip

[Psi]

It's bad practice.
And 45deg just looks nicer.

The usual arguments against 90deg tracks are..

- They act as an antenna at high frequencies, producing noise and loading your signal (there's some debate about this)
- The copper track itself can break off the pcb easier because of the small area right at the corner. 

In reality it's not going to make any difference if your circuit is simple and slow speed. Like a typical 8bit mcu or 555 timer.
But, other engineers who see your design wont be impressed.
Best to always do 45deg, you never know when you may need to show your PCB to someone, if its got 90deg tracks you probably wont get offered a job.

[sleemanj]

I would like to know if using right angle traces is a bad thing? And if so why.

For your 8x8 led matrix purposes;
  Angles less than or equal to 90 degrees are usually considered to be  aesthetically displeasing (they look naff).
  The sharp angle can create problems with etching, especially if you do it yourself, it's easier to break a trace at a sharp corner.
other than that, copper is copper (for your project's purposes).

[IanB]

I think it's the sharp corners that are worse than the angles.

[BravoV]

Check this out -> NO ! You don't need to worry about 90 degrees corner at PCB trace

If you believe 90 degrees is bad, then never use vias on your board. 

Also quoting from PCB expert :

Right angle bends do not cause signal integrity problems at any practical edge speed
Right angle bends also do not cause EMI
Right angle bends are NOT acid trap
There is no good technical reason to prevent the use of right angle bends to route traces in a PCB.

"Vias used to route signal from one layer to another do not have a significant impact on signal quality even with 200 ps edges."

[talvor]

OK, so right angle bends are a bad idea.  Cool, now I get to play around in KiCad for a few more hours 

So where should I put the 2 x 45 degree bends, close to where the 90 degree one is or further along the trace.  That is should I be trying to make the straight parts of the trace as equal as possible, or does this not matter.

[alm]

In reality it's not going to make any difference if your circuit is simple and slow speed. Like a typical 8bit mcu or 555 timer.

Low speed is up to a few GHz in this case. That's one fast 555!

[GK]

You need a nice radius to each bend, to help the electrons take the corner without flying off. They move really fast you know.

[BravoV]

You need a nice radius to each bend, to help the electrons take the corner without flying off. They move really fast you know.

Not even close, if I'm not mistaken, according to Dr. Howard Johnson at TheAmpHour session, the physical speed of the electron moving inside the conductor is even slower than a walking ant.

[marshallh]

The only electrical problem with 90 degree bends is at high speed (>100mhz) where the small part of excess copper is a minute parasitic capacitance... if you are working with stuff fast enough to worry about it, you already know the problem. At ghz speeds it becomes a waveguide and that's when you see mitered edges on the bends.

45 bends look better though.

[BravoV]

The only electrical problem with 90 degree bends is at high speed (>100mhz) where the small part of excess copper is a minute parasitic capacitance... if you are working with stuff fast enough to worry about it, you already know the problem. At ghz speeds it becomes a waveguide and that's when you see mitered edges on the bends.

Again, in the Dr. Howard Johnson session at TheAmpHour, this is also discussed and he said that at the sharp 90 degrees tip at the corner creates the same effect no more than a small lump of solder at the pcb even at ghz signal.

[marshallh]

Exactly, you'd have to route DDR3-1600 using all right angle bends for it to approach being an issue

[GK]

You need a nice radius to each bend, to help the electrons take the corner without flying off. They move really fast you know.

Not even close, if I'm not mistaken, according to Dr. Howard Johnson at TheAmpHour session, the physical speed of the electron moving inside the conductor is even slower than a walking ant.

Which species of ant? There is a lot of variation you know.

[DutchGert]

The only electrical problem with 90 degree bends is at high speed (>100mhz) where the small part of excess copper is a minute parasitic capacitance... if you are working with stuff fast enough to worry about it, you already know the problem. At ghz speeds it becomes a waveguide and that's when you see mitered edges on the bends.

Again, in the Dr. Howard Johnson session at TheAmpHour, this is also discussed and he said that at the sharp 90 degrees tip at the corner creates the same effect no more than a small lump of solder at the pcb even at ghz signal.

In my experience Dr's unsually don't know much about production.
In the past 90* corners would lead to etching problems and indeed sharp edges come of the board easyer.

In your case it's fine to use sharp edges, it's makes you just look like an absoluut n00b .

[BravoV]

Which species of ant? There is a lot of variation you know.

Ok .. ok ... I get it, must be this one ... 

The Atom Ant !!!!! 

[GK]

Years ago in high school we all had to assemble in the library one afternoon to receive a lecture in electrical safety from some supposed expert that they (school admin) managed to find from who knows where. He was an old fart and shortly after he started yacking, it became quite clear that rather than being an expert on electrical safety, he was a bit of a nutter. Spent the whole time overly enthusiastically trying to scare us, eyes bulging and arms waving and all, with exaggerated examples and stories of real life electrocutions. He concluded his spiel with an account of some bloke who got his fingers in between the joiners of an electrical extension lead - "the electricity shot right up his arm, couldn't take the corner at the top and blew his shoulder right out!". Fair dinkum. Our technical studies teacher Mr Walkley marched out of the room shaking his head. The students thought the whole lecture was totally awesome, of course, except for a few of the girls.

[Mechatrommer]

so... this $800 worth of device from Agilent is a bad practice? or they purposely intending to flew some electrons away to make the device within spec?

[GK]

An absolute poop load of old stuff was layed out exclusively with 90 degree bends - especially digital boards in the '70s full of logic chips. I'm not sure that the manufacturing/etching argument was ever that valid.
 

[BravoV]

In my experience Dr's unsually don't know much about production.
In the past 90* corners would lead to etching problems and indeed sharp edges come of the board easyer.

Also in RF designs it could lead to reflection, thats why a lot of sensitive RF designs don't like via's.

In your case it's fine to use sharp edges, it's makes you just look like an absoluut n00b .

so... this $800 worth of device from Agilent is a bad practice? or they purposely intending to flew some electrons away to make the device within spec?

I guess we will have to wait for DutchGert for that, since he boldly claims Howard Johnson and Agilent are bunch of noobs. 

[free_electron]

The only problem is manufacturability.

Acid traps is still a problem, despite what the experts claim it  no longer is.
Sure, the problem has been solved for run of the mill boards with 8 mil traces... Once you get to hdi boards it becomes a problem again. It all has to do with the thickness of the copper vs the width of the trace.  etching a 3 mil trace in 1 ounce copper is borderline. Throw in a sharp corner and the misery begins.

Sharp corners also have other problems. The soldermask is easier damaged .

That stuff all doesnt maater for your one-off board.. But for industrial production it does as it has an impact on the yield and durability of the end product.

[Psi]

Are there any advantages to a 90deg tracks that you don't get from 45deg ?
Other than maybe routing a tight corner slightly easier i cant think of any.

[Mechatrommer]

Are there any advantages to a 90deg tracks that you don't get from 45deg ?
Other than maybe routing a tight corner slightly easier i cant think of any.

you can measure traces length easier with a ruler and one eye.

[BravoV]

you can measure traces length easier with a ruler and one eye.

You're right, like in calculating the resistance across the trace in high accuracy, eg. using copper trace as low ohm resistor. 

[DutchGert]

The only problem is manufacturability.

Acid traps is still a problem, despite what the experts claim it  no longer is.
Sure, the problem has been solved for run of the mill boards with 8 mil traces... Once you get to hdi boards it becomes a problem again. It all has to do with the thickness of the copper vs the width of the trace.  etching a 3 mil trace in 1 ounce copper is borderline. Throw in a sharp corner and the misery begins.

Sharp corners also have other problems. The soldermask is easier damaged .

That stuff all doesnt maater for your one-off board.. But for industrial production it does as it has an impact on the yield and durability of the end product.

This and the fact that using 45* usually leads to shorter traces -> more free space for components or planes: win-win

Aparrently my RF story was a big load of crap as I just found out.

And ofc it simply looks nicer with 45*

[Psi]

you can measure traces length easier with a ruler and one eye.

You're right, like in calculating the resistance across the trace in high accuracy, eg. using copper trace as low ohm resistor. 

Accuracy would be better measuring that with a low ohm meter.
Rather than relying on distance measurements and assumptions about the copper thickness being exactly what it should be.

[Rigby]

I'm not very experienced in electronics, but I'm becoming somewhat of an aged fella; experienced in life.  One of the very few things that has been constant in my life is the general lack of correctness in "well known" things like this.

That is, the more people who "know" something, the less likely it will ever be verified.  Knowledge that is taken for granted is never verified.  Why would you test it, when everyone "knows" it?

Everyone "knows" that XML is far slower to read, write, and parse than plain text.  (false.)  Everyone "knows" that HTTPS is far slower than HTTP.  (false)  All sailors "know" that a snapped deck line under tension will cut you in half if it hits you.  (false.) 

I suspect this is one of those things that everyone (or almost everyone) takes for granted and never verifies, trusting the (potentially false) community wisdom over the scientific process that could prove it one way or another.

The hallmark of this phenomena is the 100% conviction shown in something that is a potential pain to test.  In software development, false community knowledge is rampant.

I'd bet that few of you who declared the 90 degree corners a bad idea have access to the RF signal generators, RF leakage detectors, or any of the necessary equipment (whatever that equipment may be) to test this, and those of you that do have access to this equipment wouldn't use it to test something "well known" like this.

I'm not arguing with anyone.  I can't tell you that any of you are correct or incorrect, because I don't know who is correct here, but I can say that this REEKS of generational knowledge that has never been tested by anyone repeating it today, and that has just as much of a chance to be correct as it does to be incorrect.

[Psi]

And ofc it simply looks nicer with 45*

I prefer nice smooth curves myself. The problem is what to do with a T junction.

This comes to mind.

[GK]

If acids traps are an issue for 90 degree bends, then why aren't they an issue for the inner corners of T junctions? Or do they have to be broadly radius-ed for ultra fine tracks? Most board houses do 6 thou track width minimum. Does anyone not laying out boards with ultra fine tracks (=> 6 thou) need to care?

Incidentally, I don't use 90 degree bends, but that is besides the point.

[c4757p]

I was under the impression that they were considered a potential issue for T junctions, hence why T junctions are occasionally seen with "chamfered"* corners.

*Not sure if "chamfer" is really the right term here, but anyway, y'all know what I mean... O0

[GK]

Well, I've never had a T junction not etch cleanly, even with 6 thou tracks. I could imagine "chamfering" the corners of every T junction on a moderately complex board being a major pain in the arse. Do any layout packages even have the capability to do that automatically? BTW, I've got Altium Designer 13 now     

[c4757p]

No idea. TBH, I've never had anything 8mil and up not etch cleanly at home in my kitchen unless I do something really clumsy. I find it a bit hard to believe that real PCB fabs would have more trouble with simple things like that than I have in my kitchen. But I have heard that.

No idea if anything can do it automatically. My instinct is that if anything can do it, Altium can... but I have no idea. One things's for sure - KiCad can't

[MacAttak]

I find it interesting that so many people have clearly stated that obtuse angles (and preferably 45 degrees) "look better" than right angles. Yet the preference was exactly the opposite in the other thread that discusses schematic wire routing.

On a schematic, everyone wants right angles. On a PCB nobody wants right angles.

However the science and reasoning behind either of those stances seems dubious at best but mostly specious?

[AlfBaz]

Would the sharp edge of a corner be a slightly better antenna thereby promoting coupling to adjacent parallel tracks like those in a multilane bus?

[free_electron]

I was under the impression that they were considered a potential issue for T junctions, hence why T junctions are occasionally seen with "chamfered"* corners.

*Not sure if "chamfer" is really the right term here, but anyway, y'all know what I mean... O0

bingo.

Code: [Select]

---   ---
    \/
     |

yes you still have a sharp 90 degree corner in the valley of the V but... the other side has a loooong trace running away , so even if you get a bit of underetching the out laying corner covers that.


now, there is another aspect : length egalisation

take a 32 bit wide bus and have it make a 90 degree corner. the outer trace will be much longer than the inner trace.
make the turn with a 45 degree angle and this changes.

[AlfBaz]

As for proving electrical issues, if I remember, the next time I get on to hyperlinx I might do a few sims and see what, if anything, pops up

[alm]

take a 32 bit wide bus and have it make a 90 degree corner. the outer trace will be much longer than the inner trace.
make the turn with a 45 degree angle and this changes.

The same will happen with two 45° corners.

[free_electron]

take a 32 bit wide bus and have it make a 90 degree corner. the outer trace will be much longer than the inner trace.
make the turn with a 45 degree angle and this changes.

The same will happen with two 45° corners.

yes, but with 45 degree corners you can often get away with only one turn.... with 90 degree corners you need two ...

[WarSim]

so... this $800 worth of device from Agilent is a bad practice? or they purposely intending to flew some electrons away to make the device within spec?

LOL look at the board!  Really look and you point will become a joke. 

[Mechatrommer]

Really look and you point will become a joke. 

clarification is much helpful. edit: "much more!" clarification is "much more" helpful.

[WarSim]

Really look and you point will become a joke. 

clarification is much helpful. edit: "much more!" clarification is "much more" helpful.

All of the critical paths use obtuse angles on the example given. 
Several of the 90deg paths required 90deg paths. 
Some of the 90deg paths functions are not obvious and most likely DC distribution and unlikely require obtuse angles. 
Only a very few could be argued to be non-critical compromises to fit the pattern. 

None of the "rules of thumb" have been obviously broken by the board shown. 

[Mechatrommer]

Several of the 90deg paths required 90deg paths. 

Really look and you point will become a joke. most 90deg traces can be converted to 45deg. they even "mixed up" 45 and 90 deg for no apparent reason. take for eg the bottom most OP07 the traces out of it is mixed (the 4 parallel traces). give me the pcb file i can convert them all to 45 deg.

None of the "rules of thumb" have been obviously broken by the board shown. 

Really read and you'll understand. i was asking if its a bad practice, regardless of anything in the world, someone argued "90deg is a noob and bad looking". not anything to do with ee or SI, its only MHz range and not fine line less than 4mil i believe as someone working with fine BGA said. so... the rule of thumb as stated by some of the posters IS broken.

[IanB]

No comment needed 

[AlfBaz]

So for length matching, would this be a definite no-no?

[WarSim]

Several of the 90deg paths required 90deg paths. 

Really look and you point will become a joke. most 90deg traces can be converted to 45deg. they even "mixed up" 45 and 90 deg for no apparent reason. take for eg the bottom most OP07 the traces out of it is mixed (the 4 parallel traces). give me the pcb file i can convert them all to 45 deg.

None of the "rules of thumb" have been obviously broken by the board shown. 

Really read and you'll understand. i was asking if its a bad practice, regardless of anything in the world, someone argued "90deg is a noob and bad looking". not anything to do with ee or SI, its only MHz range and not fine line less than 4mil i believe as someone working with fine BGA said. so... the rule of thumb as stated by some of the posters IS broken.

Yes most can be converted, I never disagreed with that.  I think we have a very different definition of "rule of thumb".   

The board was presented as an example as an obviously bad board, I disagreed.  Then again I did not research the board to determine what was a simple trace or a resistive or inductive element nor a matched pair.  Maybe we also disagree on the word obvious also. 

I disagreed, I said my piece now I stopped caring if you insult someone else's layout designs. 

[Alexei.Polkhanov]

I think something is not right here because we are talking about ways to reduce unwanted reflections but most of examples given working in range of frequencies that are waaaaaay below the point when it starts to matter.

To my knowledge it only make sense when track with is greater than 1/10 of wavelength which means that for anything less than 400MHz. Even for 900 MHz things like corners don't really matter as much. At frequencies above 4 GHz sharp corners can create reflections. ADS (Advanced Design System) for example offers curved, chamfered and mitered bends and these are separately modeled elements when moved to schematics for simulation. Angle, radius and size of track matters in this case in other words it is not just rounded - geometry has to be right otherwise it can make matters even worth. For frequencies below 200 MHz this kind of details have no effect. Someone had a photo of 200MHz active probe from HP. It is only 200MHz.

When I think about this things I always imagine a trough filled with water. Now if you have 10MHz signal on a 4 cm track it is like looking at effect of 1 kilometer long tsunami wave in 1 meter long trough. But when you observe 5mm wave in same trough you will see the reflections in the corner.

[BravoV]

Quoting Dr. Howard Johnson on his article on "Who's Afraid of the Big Bad Bend?" ...

... These models indicate that a right-angle bend has two primary effects: a slight delay plus some excess lumped capacitance. You might imagine that, as a signal traverses a right-angle corner, the trace appears to grow wider at the corner.


... For an 8-mil-wide, 50? microstrip transmission line in FR-4, the excess lumped capacitance works out to 0.012 pF. Assuming that you are using 100-psec rise and fall times, the size of the reflected signal that bounces off this capacitive discontinuity is 0.30(that's 0.003) of the incoming step amplitude. I conclude from this analysis that the reflection from a single corner is too small to worry about. (The reflected signal size scales in proportion to the trace width and inversely with rise and fall times.)


... Some people worry that conduction electrons are traveling so fast that they won't be able to make it around a square corner.  Perhaps they might reflect back or fly off into space. Such arguments are ridiculous. Sure, individual electrons move at high speeds, but their aggregate drift velocity is less than 1 in./sec as they bounce from atom to atom. Your average electron smacks into something and changes directions billions of times in a length of 10 mils. Electrons don't have any trouble banging around a corner.


... Might the electric-field concentration at a sharp, pointy corner create a lot of radiation? Hogwash.


... As digital designs push toward higher speeds, you may eventually reach a point where the right-angle bends begin to matter. For example, corners are just beginning to affect the design of 10-Gbps serial connections, and they also contribute perceptibly to skew in certain poorly routed differential pairs. If you accumulate a lot of corners, as in a serpentine delay structure, you may begin to see a little extra delay. Other than these extreme applications, right-angle bends remain electrically transparent.


... Some manufacturing engineers complain about the use of right-angle bends when using wave-soldering equipment. They worry that wayward solder balls or solder flux will get trapped in the inside corners. With reflow soldering and good solder masking, neither is a problem. I have heard no other credible negative comments about the manufacturability of right-angle bends, but I am always happy to hear from others whose experience may differ. Please write.

Read it yourself the complete writing here -> Who's Afraid of the Big Bad Bend?


Before anyone deny Mr.Johnson's argument, please, at least provide your own professional proof or "publicly" written research/experiments etc to counter his writing, otherwise, personally I will keep "blindly" trust Mr.Johnson. 

[free_electron]

So for length matching, would this be a definite no-no?

That would be a no-no, but not for signal integrity reasons. It's a no-no for manufacturability. Especially when using small geometries. If the amplitude vs repetition distance ratio is large then you will get etching problems ( amplitude is how tall the matching weave is compared to the opening between the tracks and width of track.) For a dense weave you need either chamfered or rounded turns.

Signal integrity is not affected. It is purely a processing problem. The sharp corners are prone to resist peeling when they scrub the boards . After developing the boards are scrubbed with brushes. Sharp outside edges can get damaged. Either lifting the resist or ripping it off.
During etch the outward facing corner gets attacked from both sides. This gives an underetch
If the resist was te lift during etch (we are spray etching under high pressure these days) this can give thickness variations and all kind of other problems that will cause the board to be rejected during inspection. The trace is not necessarily et hed open, it is irregular , the corner is slanted and visual inspection will fail this board as a reject. This cost money for the board fab.

So they dont like this.

Again, if you are doing 8 mil traces it is ok , but start messing around at 4 mil and below and the board house will contact you and request bot to do this, or they will increase the price as the yield goes down.

As for Mr Johnsons statement .. It is 15 years old... The world has moved on . Notice how he talks avout 8 mil traces ? Take a look at a board as made for a smartphone or a tablet. The logic board for the ipad uses 2 mil traces ... There aint a lot of room for etching variations there...

I believe johnson actually revised that statement a couple of years ago.  I need to look it up , i have the coursebook at home.

[BravoV]

I believe johnson actually revised that statement a couple of years ago.  I need to look it up , i have the coursebook at home.

Great, really eager to see that revisions. 

[Mechatrommer]

if you insult someone else's layout designs. 

ok i get it, you have a serious misunderstanding here, you cant differentiate a statement and a question mark. you've not met sarcastic type of statement yet cheers

[GK]

No comment needed 

Like I said in reply #17, though that board is really high tech, with 74LS chips rather than just 74's.

[AlfBaz]

So for length matching, would this be a definite no-no?

That would be a no-no, but not for signal integrity reasons. It's a no-no for manufacturability. Especially when using small geometries. If the amplitude vs repetition distance ratio is large then you will get etching problems ( amplitude is how tall the matching weave is compared to the opening between the tracks and width of track.) For a dense weave you need either chamfered or rounded turns.

Signal integrity is not affected. It is purely a processing problem. The sharp corners are prone to resist peeling when they scrub the boards . After developing the boards are scrubbed with brushes. Sharp outside edges can get damaged. Either lifting the resist or ripping it off.
During etch the outward facing corner gets attacked from both sides. This gives an underetch
If the resist was te lift during etch (we are spray etching under high pressure these days) this can give thickness variations and all kind of other problems that will cause the board to be rejected during inspection. The trace is not necessarily et hed open, it is irregular , the corner is slanted and visual inspection will fail this board as a reject. This cost money for the board fab.

So they dont like this.

Again, if you are doing 8 mil traces it is ok , but start messing around at 4 mil and below and the board house will contact you and request bot to do this, or they will increase the price as the yield goes down.

Thanks for the insight FE
 

[AlfBaz]

Would the sharp edge of a corner be a slightly better antenna thereby promoting coupling to adjacent parallel tracks like those in a multilane bus?

Ran some quick simulations
4/4mil track space 2ns rise times, same layer stackup, 2 tracks on top layer

The drive ends of the tracks start far away in one instance the approach is 45 deg the other 90, run together for about 0.4" and then seperate

The 45 degree approach, with a longer parallel run required 240mV threshold setting to avoid coupling indication
90 degree approach, with a shorter parallel run required 450mV threshold setting to avoid coupling

[AlfBaz]

EMI simulation also revealed higher emissions with the right angles

for the pics below
RA = Right angles
NRA = No right angles

Edit: in the pics below, ignore the lines at the top, they're different emission limits for various standards