Want some input on this board I'm working on - Page 1
Forum section: electronics / projects

author: nightfox7
author_rank: Contributor
timestamp: January 24, 2015, 12:23:25 am
content: Alright, so I'm helping out with a weather balloon project at my school and got put in charge of tracking the balloon. I'm going to be utilizing the APRS network (i'm a ham radio operator) for the tracking. There is an open source project called the trackuino, it uses an arduino in conjunction with a GPS and a radio transmitter. So normally you use a shield on top of the arduino which has the radio and GPS attached to it. I don't really like the idea of a shield because there seems to be too much room for something to wiggle loose, and I don't want to loose this thing.So i've been taking a crack at designing my own stand alone board with the AtMega328 and everything integrated to reduce the size, weight, and the chance of failure. Also, i've been learning a whole lot along the way. So if you kind people could take a look at what I have so far and give me some constructive criticism, I'd greatly appreciate it!A few things I have questions about:-I've not really grounded anything, what is the best way to go about doing that?-If there are any arduino people, does it all look kosher to you?-I've not put a reset switch, I need to do that.. Not really a question I just didn't think about it until right now.Everything i've done has been in expressPCB

author: rx8pilot
author_rank: Super Contributor
timestamp: January 24, 2015, 12:41:48 am
content: Do you have a schematic?

author: kjs
author_rank: Regular Contributor
timestamp: January 24, 2015, 02:05:08 am
content: Most ballooners I now use a complete tracker and a tiny VHF transmitter for that. That's actually the lightest and smallest thing I know of.https://www.argentdata.com/index.htmlThey have a PCB version for the tracker in SMD and a tiny SMD VHF transmitter board (MX145) which fits to it.Scott from Argentdata is into balloons and I have worked with him quite a bit.You don't need much TX power to cover a huge distance if you have line of sight. The usual big transmitters are a waste of battery power and weight.Juergen, DB3TB

author: elgonzo
author_rank: Unknown
timestamp: January 24, 2015, 03:28:25 am
content: Something looks wrong with the TO-220 package on the left side of your PCB (is it a VReg?).According to the PCB trace going from the barrel jack to the Vcc pin of the MCU, you use the barrel jack with negative polarity (i.e., center pin of the jack is ground, cylindrical contact is +Vcc). But, the wiring between the jack, the TO-220 package and those two parts on the lower left which look like electrolytic caps does not seem to be correct. As rx8pilot asked: How does the schematic of the circuit look like? Compare and verify the traces of your PCB with the wiring in the schematic...If the TO-220 is a Vreg (just my speculation), you need to connect its input with the positive terminal of the jack. Do not connect the rest of the circuit directly to the positive terminal of the jack -- since that would make the Vreg obviously pointless. Use the output of the Vreg to supply your circuit (Vcc). The two electrolytic caps are probably buffer caps for the Vreg. Choose their parameters and connect them to the Vreg as specified in the datasheet of the Vreg.Regarding GND: Use thicker traces or (preferably) ground fills/pours.Check the datasheet of the HX1 module for possible recommendations about PCB layout and try to follow them (it is probably a shielded unit, but you never know...).

author: Unknown
author_rank: Unknown
timestamp: January 24, 2015, 04:14:46 am
content: Looks autorouted? Minimal track widths, via diameters, & TH pad sizes. Part placement could be much improved e.g. the LED is 1/2 the board away from the pin that drives it, & its 220R resistor is another 1/4 of the board away.Vo & Vs of LM60 Ext. are shorted, as is the reset pin & Vcc (next to the 220R LED resistor).

author: nightfox7
author_rank: Contributor
timestamp: January 24, 2015, 05:18:19 am
content: First off I wanna say thanks for all the quick replies! I am realizing all the things I did incorrectly very quicklyI am by no means an EE or an EE student, I am a computer science major right now.Quote from: rx8pilot on January 24, 2015, 12:41:48 amI got about a quarter of the way through one and just started on the PCB, may have been unwise of me.Quote from: kjs on January 24, 2015, 02:05:08 amI was actually looking at that one and suggested that to the school, but they insisted on me building one..The HX1 radio module is 300mW, so it should be about right. I think the MX145 is slightly more powerful if i remember correctly.Quote from: elgonzo on January 24, 2015, 03:28:25 amYou are absolutely correct, I'm not sure what I was smoking when I did that.Thanks for the advice on the grounds.The HX1 is indeed fully shielded.Quote from: Tac Eht Xilef on January 24, 2015, 04:14:46 amNot autorouted, just routed by an extreme noobMakes sense to put the components near their sources doesn't it?I slapped the LED kinda as an afterthought to be honest.. i'll redo that.And yes they are.. OopsAgain thanks so much for the input, and keep it coming! As soon as I get a little bit of time I will address the problems that y'all have pointed out.What trace sizes are recommended? And via sizes?Be patient with this noob73sSeth ParkKK4QIN

author: LukeW
author_rank: Frequent Contributor
timestamp: January 24, 2015, 07:35:24 am
content: ExpressPCB is horrible... the sooner you make the move to start learning about some other software (Altium, Eagle, Kicad, whatever, any of these is better than ExpressPCB) the better.You can make the board smaller as your layout skills improve, also if you're feeling confident in layout and construction with SMDs.Here are some similar examples which might be of interest:http://rfhead.net/?p=305http://projecthorus.org/index.php/2010/06/26/new-board-update/http://projecthorus.org/wp-content/uploads/2011/09/MicroAPRS.jpg

author: nightfox7
author_rank: Contributor
timestamp: January 26, 2015, 03:45:26 am
content: Quote from: LukeW on January 24, 2015, 07:35:24 amWell maybe I will have to give the others a try. I have Eagle, but never really used it.. ExpressPCB just was easy to use.I was planning on making it through hole because the school wants it to be relatively easy to reproduce. So I figured people would do better with through hole and the parts would be more common.Those are pretty neat!-SethKK4QIN

author: nightfox7
author_rank: Contributor
timestamp: January 26, 2015, 03:49:50 am
content: Alright, I fixed those things that were pointed out earlier. Here's my revised one.Input on the groundplane is welcome, I don't know if it's the right way to do it.Are the trace sizes okay? Or should I up them? I didn't figure they needed to be huge as there is not really anything that is high current draw on here.Thanks again!-SethKK4QIN

author: kjs
author_rank: Regular Contributor
timestamp: January 26, 2015, 03:51:09 am
content: Quote from: nightfox7 on January 26, 2015, 03:45:26 amYou better learn fast how to use a different program than ExpressPCB as it will also allow you to use cheaper sources. I am using Eagle since their DOS versions so I am biased but I found that KiCAD made very good progress and has some neat features.As for through hole parts: I find that today it is usually easier to get SMD parts and I honestly mostly use SMD except for very few things. Mostly when something has to go onto a heat sink through hole is easier.Your traces are still very narrow for such a board and can lead to problems when less experienced people fry the pins in.... Your RF output connector (SMA?) also doesn't look like it was designed for 50 Ohms.....One more thing: move the voltage regulator down and the 2 capacitors up. There's no reason to connect the caps via a mile of trace even if it won't really matter.Juergen

author: tautech
author_rank: Super Contributor
timestamp: January 26, 2015, 04:02:35 am
content: Have a look at this thread:https://www.eevblog.com/forum/beginners/can-anyone-check-my-work-it-is-my-first-pcb-design/I know it's SMD but many general comments apply for you.The only thing I wish to comment on is the hole size and the annular ring. One too big and the other too small.I make holes all 25 mil then drill the right size to suit component, set an appropriate annular ring usually 100 mil, not always round

author: nightfox7
author_rank: Contributor
timestamp: January 27, 2015, 12:12:43 am
content: Okay, so I threw together a schematic in Eagle very quickly, and this is the autorouted result.. Ignore the mounting holes I have placed.The autorouter does some silly things.In your honest opinions, should I run with this one and improve it, Or just go with my older one?-Seth

author: nightfox7
author_rank: Contributor
timestamp: January 27, 2015, 12:24:31 am
content: Quote from: kjs on January 26, 2015, 03:51:09 amI threw together a schematic really quick in Eagle, it is a bit of a pain to work with but that's just the learning curve.I may up the trace size a bit and see what I can do.And from my understanding, the 5 Ohms comes from the connector and your coax correct?Thanks!-SethQuote from: tautech on January 26, 2015, 04:02:35 amCool, thats some good information!I'm still new to this so thanks for your patience.-Seth

author: tautech
author_rank: Super Contributor
timestamp: January 27, 2015, 12:47:58 am
content: Best to use the autorouter to help with component placement only.Route then look for crazy results, move components then route again and so on.Doesn't always work as intended, the router will still do silly shit sometimes, the point being that component placement to some degree must be flexible.You'll unlikely get an exceptable result with auto routers, at best you'll need to modify the result in numerous ways.

author: nightfox7
author_rank: Contributor
timestamp: January 27, 2015, 01:21:20 am
content: Quote from: tautech on January 27, 2015, 12:47:58 amAh okay.. Well I don't know I did something wrong or what, but the component placement was pretty crappy when I made the PCB from the schematic in Eagle.. I rearranged everything with how it is in that example.Here's an updated view of what the one that i'm working on in expressPCB looks like now. I increased the trace size, the pad size, and rearranged a few of the components. Ignore the Ground that isn't connected on the radio.All the pads are 1.57mm and the holes are .74mm.

author: elgonzo
author_rank: Unknown
timestamp: January 27, 2015, 01:29:59 am
content: I do not know how much heat the Vreg will dissipate, but it is probably not such a good idea to place the Vreg so close to the electrolytic caps, which usually don't like getting all hot and cozy. If you are sure that the Vreg does not get very warm, then it is of course okay to keep the caps very close to the Vreg.

author: tautech
author_rank: Super Contributor
timestamp: January 27, 2015, 01:41:43 am
content: I'll not tell you how to do everything, there is plenty to learn for youelf.CommentsYou seem to have plenty of room so spread things out a little.Rotate E caps 90Move VCC trace further way from headersTry to enter all pads at right-angles.(not vias)Attempt to create all traces as either horizontal, vertical or 45 degreesResist (not don't) running traces between device pinsThink carefully of PCB population and soldering order and throw possible re-work needs also to component layout. (shit I can't get to that component without removing 3 others first.)Needless to say you're coming along.

author: JE
author_rank: Newbie
timestamp: January 30, 2015, 06:14:01 pm
content: I've used ExpressPCB for many years, I like how quickly you can throw a board together, the software is to use and prices aren't too bad, I still use them for prototyping.I will add you should NEVER use auto-router! I believe it would over complicate a 2 resistor board layoutI didn't look over the entire board, but this jumped out at me and I pointed it out on your latest board, just follow the trace.

author: nightfox7
author_rank: Contributor
timestamp: February 03, 2015, 07:43:12 pm
content: Quote from: tautech on January 27, 2015, 01:41:43 amThanks!I don't expect anyone to do my work for meGreat tips, I'm still catching myself doing idiotic stuff it seems.Here's the latest revision of the board.Quote from: JE on January 30, 2015, 06:14:01 pmHaha i just made a completely unnecessary trace. I am redoing it in Eagle so i can get it manufactured by other companies.on that note, opinions on OSHpark?

author: tautech
author_rank: Super Contributor
timestamp: February 03, 2015, 08:53:47 pm
content: I'd much prefer to run traces out the ends of an IC then between pads when possible.Have a took at those that you can. There are a few.For other than high speed lines, a longer trace will not matter much.One or two traces on the other layer can make ALL the difference to tidy routing.TH passives are especially valuable for "roadways" for traces.Arrange them to make the gaps.Autoroute to check....undo...rearrange.... autoroute....undo and so on.Manual Route to finish.Try to keep traces further away from pads if possible. Yeah I know thats where the autoroute puts them....change the clearance rules or manually move them.If you do a board without an overlay or solder mask, you'll be thankfull of more clearances.Think solder bridges.

author: EK701
author_rank: Contributor
timestamp: February 03, 2015, 10:10:25 pm
content: Why are you running a trace under R8 to R11? Err outing around it will give you more clearance for the trace that does go to R8. I would also rotate R8 180 degrees. The routing to pins 2 & 5 on SPCI could be cleaned up. Drop the component values from the board. Clean up the component names. What tautech said on pad clearances.I've used OSH Park on numerous occasions and have been satisfied. Their boards are quality.