Following is from a PCB that I am presently working on. That particular path signals are of 100-400kHz signals. Is there any problem in having routes of this kind?
Electronic – Acute angle routes in PCB
eaglepcbrouting
Related Solutions
The Eagle autorouter is a decent tool, and I use it a lot. However, like any tool, you have to know how to use it well and understand its limitations. If you are just expecting to throw everything at the autorouter, you will be dissappointed. No current auto router, and probably for a number of years to come, can do that for anything beyond contrived or toy problems.
You say there are settings in the Eagle autorouter you don't understand and never mess with. This is a bad attitude, and probably a good part of your problem. There is no set of control parameters that works on all boards. Even within 2 layer boards there are various tradeoffs. You absolutely have to read the manual and adjust the parameters for your particular situation.
For two layers boards, I often try to keep most of the bottom layer a ground plane. I therefore use the top layer for interconnects as much as possible, and the bottom layer for short "jumpers" to make the routing topology work out. In this case, I set a high cost for routing in the bottom layer.
Before autorouting, you have to look at the board and think about the critical areas that you can't explain to a autorouter. For example, you want to keep the loop currents of a switching power supply local and off the main ground plane. The same holds true for high frequency currents local to a digital chip, like bypass caps and crystal with its caps. If you are using the pseudo ground plane layer as I described above, then you want to manually connect every ground connection immediately to the ground plane with its own via. That leaves maximum room on the top layer for routing everything else.
The process of routing a board even when letting the auto router do most of the grunt work looks like this:
- Manually route the critical paths, as I mentioned above.
- Do basic housekeeping pre-auto routing. This includes connecting all the ground pins directly to the ground plane for example.
- Look for problem areas where you can see the autorouter might get itself into trouble. If there are short connections in dense areas you might want to make some of them. This takes some experience and intuition, so if you're new to the particular autorouter, skip this step for now.
- Save a copy of the board, then run the auto router. If this is the first thru here, just have it do the minimum to find a solution. The purpose of the first few times is to see where the problem areas are so you can adjust the layout and your manual pre-route accordingly.
- Look carefully at the resulting route. See where the problem areas are. Revert back to the saved copy from step 4 and adjust your layout and manual pre-route according to what the auto router did. Repeat back to step 4 until the result looks reasonable. As you do more iterations thru here, you crank up the autorouter optimizations and other parameters to make a more final route. In the beginning you are just trying to see if it can find a solution and what the large problems are. In later passes you converge on a real route. I start out with no optimization passes, and use 8 for final routes. I also configure early passes to find a solution, then later passes to optimize it.
- Do manual cleanup on the route. In the case of a two layer board with mostly ground on the bottom, you want to minimize the maximum dimensions of islands in the ground plane. It is better to have a large number of small islands than fewer large islands. Sometimes you can see ways of rearranging signals locally to minimize the jumpers on the bottom layer. In this stage, the big picture has already been taken care of and you are focusing on manually optimizing small areas. This is similar to a peephole optimizer of compilers.
Here is a Eagle autorouter control file I used on a two layer project with the bottom layer a ground plane to the extent possible:
; EAGLE Autorouter Control File [Default] RoutingGrid = 4mil ; Trace Parameters: tpViaShape = Round ; Preferred Directions: PrefDir.1 = * PrefDir.2 = 0 PrefDir.3 = 0 PrefDir.4 = 0 PrefDir.5 = 0 PrefDir.6 = 0 PrefDir.7 = 0 PrefDir.8 = 0 PrefDir.9 = 0 PrefDir.10 = 0 PrefDir.11 = 0 PrefDir.12 = 0 PrefDir.13 = 0 PrefDir.14 = 0 PrefDir.15 = 0 PrefDir.16 = * Active = 1 ; Cost Factors: cfVia = 50 cfNonPref = 5 cfChangeDir = 2 cfOrthStep = 2 cfDiagStep = 3 cfExtdStep = 0 cfBonusStep = 1 cfMalusStep = 1 cfPadImpact = 4 cfSmdImpact = 4 cfBusImpact = 0 cfHugging = 3 cfAvoid = 4 cfPolygon = 10 cfBase.1 = 0 cfBase.2 = 1 cfBase.3 = 1 cfBase.4 = 1 cfBase.5 = 1 cfBase.6 = 1 cfBase.7 = 1 cfBase.8 = 1 cfBase.9 = 1 cfBase.10 = 1 cfBase.11 = 1 cfBase.12 = 1 cfBase.13 = 1 cfBase.14 = 1 cfBase.15 = 1 cfBase.16 = 5 ; Maximum Number of...: mnVias = 20 mnSegments = 9999 mnExtdSteps = 9999 mnRipupLevel = 50 mnRipupSteps = 300 mnRipupTotal = 500 [Busses] @Route Active = 1 cfVia = 10 cfChangeDir = 5 cfBusImpact = 4 cfPolygon = 25 cfBase.16 = 10 mnVias = 0 mnRipupLevel = 10 mnRipupSteps = 100 mnRipupTotal = 100 [Route] @Default Active = 1 [Optimize1] @Route Active = 1 cfVia = 99 cfNonPref = 4 cfChangeDir = 4 cfExtdStep = 1 cfHugging = 1 cfPolygon = 30 cfBase.16 = 10 mnExtdSteps = 20 mnRipupLevel = 0 mnRipupSteps = 100 mnRipupTotal = 100 [Optimize2] @Optimize1 Active = 1 cfNonPref = 3 cfChangeDir = 3 cfBonusStep = 2 cfMalusStep = 2 cfPadImpact = 2 cfSmdImpact = 2 cfHugging = 0 cfPolygon = 40 mnExtdSteps = 15 [Optimize3] @Optimize2 Active = 1 cfVia = 80 cfNonPref = 2 cfChangeDir = 2 cfPadImpact = 0 cfSmdImpact = 0 cfPolygon = 50 mnExtdSteps = 10 [Optimize4] @Optimize3 Active = 1 cfVia = 60 cfNonPref = 1 cfPolygon = 60 cfBase.16 = 12 [Optimize5] @Optimize4 Active = 1 cfVia = 40 cfNonPref = 0 cfPolygon = 70 cfBase.16 = 14 mnExtdSteps = 5 [Optimize6] @Optimize5 Active = 1 cfVia = 20 cfBase.16 = 16 [Optimize7] @Optimize6 Active = 1 cfBase.16 = 18 [Optimize8] @Optimize7 Active = 1 cfBase.16 = 20
I'd like to chime in with a bit of perspective: you're not really dealing with anything high speed here. You can really do whatever you want at these frequencies and get perfectly fine signal integrity. A couple of MHz, even a couple tens of MHz, won't cause any real trouble.
Especially on the crystal side of things, you don't have to worry about a thing. I've had layouts where the crystal was placed several inches away from an MCU, and it worked just fine. I probed it, it looks just like the crystal is tightly coupled. High speed design is 300MHz and up - or high impedance from about 100MHz. That is roughly the point where routing can start causing clock skew, reflections and where your PCB traces won't behave as resistive elements anymore.
In any noise-sensitive design, you want to consider that:
- Electric fields and especially their rate of change should be minimized. Electric fields are proportional to voltage and inversely proportional to distance, so you want to maximize spacing between lines that swing their voltage rapidly
- Magnetic fields should be minimized. Magnetic fields are proportional to loop size and rate of change of current, so you want to decouple anything that has a high rate of current change (power conversion, IC power lines) with suitable capacitor values and you want to route power lines as closely together as possible to minimize the size of the current loops
- High impedance means low noise immunity. Avoid high impedance lines, and if you have them, make them as unsusceptible to noise as possible. Shield them, guard them, but ideally just terminate them with a low impedance so you don't have to deal with it.
Related Topic
- Electronic – Eagle: Pins on FPGA exchangeable, depending on configuration
- Electronic – Four layer PCB power plane
- Electronic – What are some tips to routing a one sided PCB
- Electrical – Eagle’s PCB ratsnest command reports 3 airwires, but they are not visible
- Electronic – Route crossovers on PCB routing
- Electronic – ny PCB design software/extension that can do automatic components placement
Best Answer
Old timers might grumble about "etchant traps" ... acute angles can hold acid (well, FeCl) long enough to eat through the track - or not, depending on who makes the PCB for you. Consult with them if you are worried.
But I was downvoted for pointing that out in a previous answer, so at least somebody thinks that's no longer a problem.
As far as the signal speed on that trace - nothing to worry about.