I am just wondering if it is possible to get a trace out from the inside teensy pads without running into problems. The bads are very close together so it involves making traces go in between pins that are 2.54 mm apart. I am wondering if this is possible/ has anyone done this. I tried with a board I etched and when I would set a pin high, certain other pins would read as high as well. I did do this without a ground plane so I think that may be part of the problem, I am just wondering if anyone has done this. Thanks for any info.
Getting traces between teensy pins.
- Thread starter mcsteeze
- Start date
- Status
PaulStoffregen
Well-known member
It depends on the PCB specs. If you use OSH Park, the specs are 6 mil traces and spacing. You can easily get two traces between the pins, 12 for the traces and 18 for the spaces still allows the pads to be up to 70 mils in diameter.
For a home etched board, it really depends on how good you process is. When I used to etch boards, I could usually go down to 10 mil traces, but 15 or 20 worked better. I needed only 10 mil spacing, since the acid usually etched the traces thinner. That was a photoresist process. If you're using iron on transfer or some other way, what type of traces and spacing you need can be quite different.
For a home etched board, it really depends on how good you process is. When I used to etch boards, I could usually go down to 10 mil traces, but 15 or 20 worked better. I needed only 10 mil spacing, since the acid usually etched the traces thinner. That was a photoresist process. If you're using iron on transfer or some other way, what type of traces and spacing you need can be quite different.
Thanks for the answer.
Have you ever had a problem with capacitive coupling when (home etching) and having a thin trace so close to the teensy pins? This is why I have been trying to home etch 6 mil traces (to leave as much space between the traces and the pins), rather than going with 8 or 12 mil traces.
I etched my own board, and when I set some of the pins high, frequently the pins next to that pin will read go hi too. I am wondering what is causing this.
Have you ever had a problem with capacitive coupling when (home etching) and having a thin trace so close to the teensy pins? This is why I have been trying to home etch 6 mil traces (to leave as much space between the traces and the pins), rather than going with 8 or 12 mil traces.
I etched my own board, and when I set some of the pins high, frequently the pins next to that pin will read go hi too. I am wondering what is causing this.
PaulStoffregen
Well-known member
Maybe they're shorted together? Did you try measuring the resistance between them with a multimeter? With the power off, the tiny test current from the meter will flow through the ESD protection diodes in the chips, so you'll see measurements like 100K to 5M (depending on the design of your meter), rather than a truly high impedance. PCB shorts are things like 0 to 100 ohms.
I just tested most of the pins with a meter. I already had tested them in continuity mode, and none of theme beeped with a short. I then retested with my meter on the 20 Mohm (highest) setting. Many of the pins close together we reading in at .67 and higher (I believe that is 670,000 ohms). Could that somehow be the cause of my issue?
For one thing, this board I made does not have a ground plane, I am curious if the ones you used to make did, and any steps you took (with 15 mil traces and 2.54mm dist between holes) to prevent shorts and capacitive coupling.
For one thing, this board I made does not have a ground plane, I am curious if the ones you used to make did, and any steps you took (with 15 mil traces and 2.54mm dist between holes) to prevent shorts and capacitive coupling.
adrianfreed
Well-known member
Are you cleaning the boards carefully? Flux, oil from your fingers etc. can easily result in 670KOhm measurements?
Would 670Kohm cause a short do you think?
I have cleaned the board quite carefully. There could be several issues, I am just trying to figure out if it is possible to get a trace between the pins without an amount of capacitive coupling that prevents a good connection.
Is the 670 Kohm measurement bad? Would that classify as high impedance?
Epyon
Well-known member
You can't measure capacitive trace coupling with
a) the microcontroller still plugged in
b) a multimeter (this only measures DC resistance).
To measure capacitive coupling, you need to apply a high frequency signal to one trace and measure the other traces with e.g. an oscilloscope.
Keep in mind that capacitive coupling is not necessarily a problem, because while it can lead to a high potential on another trace, the amount of transferred power is very low. Capacitive coupling is mainly a problem for analog sampling, less for digital signals (except on high frequencies). You should always use pull-up/down resistors when using relatively long digital lines on relatively low frequencies, which will remove this problem.
I regularly route traces between 2.54mm pins without problems, even on a board using a Teensy. Ofcourse, you need to put some effort in routing and laying down your ground planes
.
a) the microcontroller still plugged in
b) a multimeter (this only measures DC resistance).
To measure capacitive coupling, you need to apply a high frequency signal to one trace and measure the other traces with e.g. an oscilloscope.
Keep in mind that capacitive coupling is not necessarily a problem, because while it can lead to a high potential on another trace, the amount of transferred power is very low. Capacitive coupling is mainly a problem for analog sampling, less for digital signals (except on high frequencies). You should always use pull-up/down resistors when using relatively long digital lines on relatively low frequencies, which will remove this problem.
I regularly route traces between 2.54mm pins without problems, even on a board using a Teensy. Ofcourse, you need to put some effort in routing and laying down your ground planes
.Does this mean it would only be a problem when I am reading analog pins?
I have traces that are about 4.5 inches long and are thin (about 7 mils or so). I do use pull-ups but do you think that that distance could create some problems witht he readings?
I regularly route traces between 2.54mm pins without problems, even on a board using a Teensy. Ofcourse, you need to put some effort in routing and laying down your ground planes
Given the scenario I described above, how necessary is a ground plane? (Or Just in general how necessary are they would you say?). Thanks
Epyon
Well-known member
No, but it's mostly a problem with analog readings. However, when you don't use pull-up/down resistors on your digital lines, it will cause problems there too. Digital pins configured as digital input are in a high impedance state, meaning they require almost no current to detect a logic high. Floating input pins will randomly show up as high or low, because capacitive coupling is enough to supply this very low current.
While you can almost always use pull-up/down resistors on digital pins, you should be able to circumvent this problem. However, it's much harder to use these resistors on analog lines because it can lower the input impedance of the measurement circuit, disturb the circuit under test, cause ADC input impedance mismatch etc. That's why analog sampling is more sensitive to this interference.
My smallest traces are 10 mil, which is thin enough to route between 2,54mm headers, with some of them having lengths of up to 70mm. Don't really have problems, but of course i don't know on which speeds you work. I only use LF signals, not much more than a couple of kHz's at most (except SPI, which runs at 4MHz).
Anyway, whole lectures can be given on trace width and routing. E.g. making your traces wider can increase the capacitive coupling because there is more surface that can act like a charged plate. You can also have inductive coupling, especially on traces carrying power (e.g. digital drive pins). The whole crosstalk problem is dependent on trace geometry, trace length and distance, ground plane position, dv/dt of the signal, the dielectric constant of the PCB material etc. Fortunately, for LF signals you don't have to worry too much about this.
I always use some basic tricks in my PCB design, one being an adequately laid down ground plane. This is mostly to provide all components with a low impedance ground path, because i find a lot of problems on LF boards are caused by inadequate grounding. When using a ground plane, or just whenever you lay down ground traces, you need to make sure the current only has one 'way' to flow to the ground plane or the ground connection. When you use multiple connections you run the risk of creating circulating currents in your ground connection, leading to common mode problems.
I also always use a separate ground plane for analog components, which is connected to the main ground plane through a single trace. This ensures noise, circulating currents and common mode problems stay out of my analog section.
Thank you. I am designing my boards using Fritzing which has an automatic setting for copper ground fill (I am not exactly sure how it works). My only issue is that I have a few pins that are not routed to anything, and a couple pins which are going to be routed to external sensors (i.e. not on the pcb). I've never used a ground fill before but it looks like the right choice here.
Thanks for your help.
Thanks for your help.
- Status