JTAG wiring diagram question « LeafLabs Garden

LeafLabs Garden » Support » Maple Hardware Support

JTAG wiring diagram question

(63 posts) (9 voices)

Started 5 years ago by Adam
Latest reply from gbulmer

« Previous 1 234 5 Next »

Adam
Member

gbulmer,

Thank you for all the improvement suggestions!

I will make them in my next board rev, after I get the first batch back.

Re: the copper pour, good idea. I did try to do one last night, but could not figure it out in time to get my boards in to the run. I will see if I can figure it out next weekend.

Re: the SIL, I am actually hoping to remove all but three of the resistors since the STM32 has internal resistors. When I get the ARM-USB-OCD I will see if that works. If it does then the board could be quite small even with through-hole resistors.

Re: jaggies in the PNG image - I looked at the gerbers in gerbv, and there are no jaggies there. I think the PNG looks funny due to rasterization.

Re: lining up components better and using wide tracks, I will do that in the next rev. I did have a hard time getting components lined up because of the lack of guidelines... the Eagle grid leaves something to be desired.

Re: layers, I will see if I can make those changes. If I can remove most of the resistors it will be easier. I will also see about rearranging things to make the signal paths more understandable.

soundcyst,

Re: rules file, I did use Laen's rules file.

Re: mitering, I used 45 degree miters to avoid right angles. I did try to keep things to horizontal, vertical, and 45 degrees... but perhaps the angles are slightly off. I will try to fix in the next rev.

Re: messy, how would you clean it up?

Posted 5 years ago #
soundcyst
Member

i'm having a look at this in eagle now instead of just the png.

some of the "keeping it clean" stuff has a lot to do with your eagle workflow.. a good workflow will make it easier to maintain good habits. whenever i start with a completely unrouted board, i always hide the power and ground signals using "rats ! gnd" and "rats ! vcc".

(as an aside, when i say "signal" below, i don't mean power or ground. eagle uses the word "supply" to refer to these types of signals.. the words are a bit overloaded, but hopefully that makes sense)

first, move the resistors so you keep the trace lengths as short as possible. keeping signal traces short isn't really crucial unless you're doing high speed design, but it does make routing easier. supplies don't necessarily need to be short, and typically (in high speed boards anyways) you have a whole plane for the supplies.

r7, r8, and r9 are good examples. one side is connected to supply, and one side to signals. the signals should be as close as possible to the 20 pin connector. rotating all three of these 180 degrees makes routing easier, and when you have the power and ground ratsnests hidden, this becomes a bit more obvious.

one of my biggest grievances with eagle is that it doesn't lock traces to angles (it's a blessing and a curse really, but more of a curse). orcad does, which is really pleasant, but it's about an order of magnitude more expensive, and there's no free version, so it's a pain we have to live with.

so, even if you're using the 45 degree route tool, if you move a part, suddenly the angle is no longer 45 degrees and you have to move the trace as well.

it also sounds like you're confusing mitre and angled routing. mitring actually rounds the edges, and based on the files i cloned, it looks like you didn't do any mitring. this is ok, as mitring isn't really necessary, it's just good practice.

another thing is getting eagle's grid to work for you instead of against you. part of this is personal preference, but part of it is learning your options so you can be educated in your preferences. personally, i use 0.01 as my main grid, and 0.001 as my alternate grid (both in inches), which keeps things organized for the most part, but allows me precision when i need it.

i'll do a few things to this and post it on git or as a zip file here..

Posted 5 years ago #
soundcyst
Member

ok, are we all sure this schematic is correct? R1 and R6 overlap each other completely in the schematic to the extent that it looks like only one resistor. something tells me this is an error. TDO is probably not required to be pulled up by two 10ks in parallel..

edit -- here, assuming there's only supposed to be one pullup there,
https://github.com/soundcyst/maple/blob/master/jtagadapter/maple-jtagadapter-brd-xkn.png

(fair warning: i didn't run the dru on that, so there could still be some design errors)

Posted 5 years ago #
gbulmer
Moderator

adamfeuer -

I will make them in my next board rev, after I get the first batch back.

I guess my British understatement is causing problems, and not helping.

Let be be clearer.

PLEASE do NOT make the PCB design you posted.

I hope that soundcyst and I have helped explain some reasons for that suggestion.

Of course, if Laen won't pull the design and let you replace it, just let it go.
IMHO, with a few hours, the design could be as good as it'll ever need to be.

Posted 5 years ago #
gbulmer
Moderator

ok, are we all sure this schematic is correct?

I am not. An image of the board was posted without a schematic to match.

Let me pull the ECAD down, and have a look.

I notice you spun the 10x2 socket 180 degrees, and it does look much simpler.

Posted 5 years ago #
soundcyst
Member

the schematic is in the git repo that adam linked. (and also in the official leaflabs/maple repo) by "we all" i was meaning to include some of the leafblowers as well (mostly okie, since he drew the schematic).

and yeah. spinning the socket helped a lot.

Posted 5 years ago #
gbulmer
Moderator

R1 and R6 overlap each other completely in the schematic to the extent that it looks like only one resistor. something tells me this is an error.

I see it. Yes, that looks like an error. It isn't a disaster because one of the two resistors can be left off the board, but it looks like an error.

another thing is getting eagle's grid to work for you instead of against you. part of this is personal preference, but part of it is learning your options so you can be educated in your preferences. personally, i use 0.01 as my main grid, and 0.001 as my alternate grid (both in inches), which keeps things organized for the most part, but allows me precision when i need it.

I strongly agree. Everything gets much easier if the grid is used to help.
For a board on a 0.1" grid (which this mostly is) I would set the main grid to 0.05", and alternative to 0.005" or even 0.01" because there isn't much that is likely to benefit from anything finer!-)

The track width is 8mils, i.e. 0.008".
IMHO that is much finer than necessary. That is about 0.2mm.
The board would be okay with 0.4mm or even wider. The wider tracks will be okay to solder, and likely remain undamaged if parts need to be desoldered.

The whole board is offset from the origin. Not a big issue. I'm unsure, but it might cause extra work when someone tries to panelise it.

Many of the parts are not on a consistent coarse grid, i.e. 0.05", so the tracks have got stepped edges within Eagle.

soundcyst - I've just had a look, and I think your layout is better than mine.
I left a gap between resistors to make them easier to stuff.
Your routing lends itself to a SIL resistor array or two :-)

The only change I would make to your routing is the connection between the 20-pin header's pin 3 and 15, and maybe use the wider track for ground (that's not on here).
I'd route 3 to 15 between the two rows of pins, then it pops up onto the top layer.
Of course, the missing ground needs to be routed, but it is pretty clear that will be clean.

Then copper pour to create ground planes top and bottom, and its done.

Nice work soundcyst.

Edit - oops, our posts crossed while I was laying it out too :-)

Posted 5 years ago #
gbulmer
Moderator

One thing I forgot to say is I always look at, and preferably print, the PCB out as near actual size as I can.

I find working on the zoomed images all the time misleading, and a bit seductive.

When I look at it at actual size, it become clearer to me whether or not it looks okay.
Fine tracks just disappear.

Now, looking at that, I think I'd need to see the resistors to feel comfortable about the tighter, 0.1" spacing of the resistors.
I have some 10K resistors hanging around that are a bit too big for 0.1", and would be easier on 0.15"
Not a big issue, but I was a bit surprised how small it looked when it was at actual size.
(Having said that, I'd prefer to use two SILs :-)

Posted 5 years ago #
Adam
Member

soundcyst, gbulmer,

Wow, thank you for all the help!

I will see if Laen will let me swap out the board layout. We should do that sooner rather than later, though.

soundcyst's board layout looks better than mine. However - on the schematic, the odd pins on the 20 pin ARM-JTAG connector are unconnected, except for pin 19. The trace from pin 19 goes through pin 20 and connects to pin 7 on the Maple JTAG, VCC. However, on the schematic, 20 goes directly to ground, not to VCC.

Or am I missing something?

Re: moving the resistors to allow more space - soundcyst, do you agree? If so, would you be willing to do that?

Also - who will do the copper pour? soundcyst?

Re: mitering, well, I used the Eagle miter tool, set to angled miter; should I have used curved miters?

If you don't have time to do it - I can try it tonight after dinner or tomorrow night, let me know.

Posted 5 years ago #
gbulmer
Moderator

I will see if Laen will let me swap out the board layout. We should do that sooner rather than later, though.

Agreed. Maybe ask him if you can have a day to fix it?

... However - on the schematic, pins 4,6,8,10,12,14,16,18, and 20 are directly connected to ground. On this board, they are left unconnected.

You are correct, maybe when soundcyst hid the ground airwires, it was left unrouted.

It should only take 15 minutes to fix as the routing is very direct.

I am very sorry to desert you, but it is 2:30 am here, and I need to get up early to get ready for a little workshop I'm running in the (later:-) morning.

The ground polygon is literally: draw a polygon with quite a wide track, say 0.024 wide around the edge of the board, top and bottom. Do it by selecting polygon, then clicking, say, top left corner within the board, then bottom right (for two sides), then close it be returning to top left and double click.
Chage the name of the polygon to GND. Hit ratsnest, and it will calculate the copper pour. Do the same on the other layer.

Try to ensure their is a margin with no copper around the board, it is possible ot get small filaments of copper, if the copper extends to the edge, when a board is cut, so leave a margin (shouyld be in the design rules).

Sorry to run, I won't have much time to help for about 20 hours.

Posted 5 years ago #
gbulmer
Moderator

Ooops - have a look at the PCB printed actual size. The resitors may be fine, in which case their is only the grounf routing and copper pour to do.

Night.

Posted 5 years ago #
soundcyst
Member

looks can be deceiving.

the screenshot i posted doesn't show the pours filled in, but they are there. if you look closely to the bottom, the dotted blue and red outlines are the pours.

>>Or am I missing something?

sortof. there is one big big error with what i posted, and that's that the labels 1 and 20 are now in the wrong place and should be swapped. as gbulmer mentioned earlier, i rotated the connector, but i didn't move the numbers.

i'm not sure where okie came up with this schematic, but if you look at this ST document at the bottom of page 19 they have a schematic from arm 20 pin to the relevant pins on the stm32, and they're only using 3 pulldowns.. that prompted me to check the reference manual, which indicates that NTRST, TDI, and TMS are all pulled up internally. TCK, which is pulled up in okie's schematic, is pulled down internally, which means there's some power waste there, and probably also Bad Things (TM).

so, i would remove all of the pull ups and go by the schematic from the above link. but, it would also be helpful to get an okie's input just for clarification.

>> Re: moving the resistors to allow more space - soundcyst, do you agree? If so, would you be willing to do that?

i would rather encourage you to do it yourself! ;)

Posted 5 years ago #
gbulmer
Moderator

soundcyst - Couldn't get to sleep, something bugging me.
Realised copper pour would connect GND, D'oh!
Remembered hardware design, getting started, app note (looking at yesterday for power, amazing decoupling capacitor structure), and slightly remembered JTAG D'oh!
Retrieved laptop (it is -6C here, so not pleasant) ...

... and here you are :-)

(In the interest of full disclosure, I remembered the schematic, but I didn't remember *any* of the written JTAG details).

It does look like the JTAG schematic in the Maple repo should be expunged, with extreme prejudice.

While I am awake ...
I remember seeing a power supply schematic, which I believe was for the STM32F, which had an inductor. I've looked a bit but not found it again. Does anyone else remember seeing that schematic?

Night night.

Posted 5 years ago #
Adam
Member

soundcyst said:
> i would rather encourage you to do it yourself! ;)

I am working on it now!

As for which schematic to follow - yeah, there's a matching schematic for the STM32 ARM JTAG in the STM32 reference manual. But I'm going to follow okie's schematic (minus the extra resistor), since he has a working jtag adapter and told me he took the schematic off his board. I had a conversation with him on IRC the other night about this...

If this board works for me - then I will try removing the other resistors on my breadboarded adapter and if that works, on the next run of boards.

Posted 5 years ago #
structuresound
Member

I have a working adapter that I made with an 8-pin header soldered to pins which I shoved into the 20pin header on my Olimex. It's a pretty trivial thing to make so I don't really understand the need for a PCB unless it's something the leaf blowers wanted to add as a "stocking stuffer" to those interested in J-tag. Don't let me be a "nay" sayer though, a good PCB would save some folks some heart-ache I'm sure.

Posted 5 years ago #

RSS feed for this topic

« Previous 1 234 5 Next »

Reply »

You must log in to post.