Amega328p-au shorted pins ?

Question

Finally motivated myself into trying Eagle files only to see my original instincts told me NOT to bother.

The last thing I expected was not finding common components in the library.My first mistake to assume that an Atmega328p-au would be one of the easiest to find.Not so and had to search the ends of the earth to find it and manually place it into the LIBR directory.After a 4 hour search and finally having this IC in my schematic layout I now see"shorts on several pins of this chip in the BRD window.The worse possible places no less on 3.3v and ground

I can probably modify this file but now getting far deeper into a simple project I thought would be straight forward.

Is it a software glitch causing this or a bad library file ?

Anyone know where to find a working Atmega328p-au footprint

See attached screen shot of the issue.

n2nxz · Answer

Been some time and have made great progress with help from this group.

Thanks to Rachel and others for your patience and help.

I have since taken a long break from these circuits but had a lot of fun and interesting flights using them.

My last PCB was much smaller a friend shared with me and almost flew it around the earth twice.It lasted 63 days in the sky floating all over the world.

I am posting this as I share this with others also wanting to design,build and fly these projects and hope they get something from it.

https://www.qrp-labs.com/flights/u3s22.html

Jim

n2nxz · Answer

Just for FYI,a website was started with details of this circuit and hobby - radio-signals forum – radio-signals.com Jim

rachaelp · Answer

Paul Ellison wrote: Only just today I have downloaded the latest version of Eagle (for Mac) and attempted to create parts for a new design. Unfortunately the library editor seems to continually crash. It seems to be a known issue: https://forums.autodesk.com/t5/eagle-forum/editing-device-crashes-eagle-8/td-p/6879433 I would recommend you stick with version 7.7. At least for now. I'm going to have a look at KiCad. Yes, license issue aside (I don't want that to kick off in this thread too!), it seems the 8.0.x releases are not fit for purpose at the moment. I've had numerous crashes and the latest v8.0.2 seems to have the most dysfunctional library editor yet.... Fortunately I have a 7.7 Ultimate license which I will be sticking with until such time v8 works reliably and they have some worthwhile new features. Best Regards, Rachael

n2nxz · Answer

All my problems are because of Windows XP C++ library issues and always no solution.Been down this road 100`s of times and this happens with some programs and not others.Not going to waste my life on fixing it. However,installed the latest version of Eagle onto a newer laptop here,transferred my new LBR files and first shot everything works like it should. Going to get to work,enough time wasted already. Thanks for those who tried to help and maybe this posting will help someone in the future rather than wasting time. Jim

rachaelp · Answer

Hi James, I've just had a quick look at your latest schematic and made a quick board with it. The first thing to note is that your silk screen elements in the board your a mixture of vector (correct) and proportional (incorrect) and this will lead to your silk screen on your PCB not looking like you expect when you get your boards back. To have clear and consistent silk screen legends which match the board you must you vector for all your parts. Now, this isn't your fault exactly, its down to relying on poor quality parts sourced from either the bundled "free" libraries or from the internet. Now, onto your DRC problem. When I ran your schematic through to a board and ran DRC, if I don't load a .dru file from the board manufacturer and rely on the defaults, then I get a bunch of clearance errors. I then went and loaded the basic 2-layer .dru file from Eurocircuits and ran DRC and it passed without error. What fab house are you using for your boards? Do they provide an EAGLE .dru file (or files) for their capabilities? If so then load this and run DRC. Then if there are still any errors, examine them on a case by case basis to determine if you really need to worry. With regards the auto router, well you can use it if you must but you wont get the best result. I think it's best used as a tool to help manual routing. Manual is the way to go really and then you can use the auto-router selectively to help you route simple but very repetitive groups of traces. First thing to do though it to get the placement right as that is 90% of the battle. Move things around, rotate etc, even update the schematic if needed to get the air wires to run a cleanly as possible. Remember to run ratsnest regularly so you can see how things are improving. Once you are happy with placement you can then start to route things in. I get critical nets like clocks routed in first, then work your way through the rest, leaving the least critical to last. Make sure your power and grounds are done well and do make sure you have adequate decoupling caps. I don't see any bulk or bypass caps in your design. I know you are trying to save weight but you might need a few. internal power/ground planed in the board will help there too, although again they will add a little weight. Best Regards, Rachael

rachaelp · Answer

Hi James, I'm glad you are learning and making progress Hopefully you are finding it more rewarding now you are starting to see some results. I just had a quick peek at the two images you posted up. I have a couple of comments. Firstly, your power net is routed around the board with a really skinny trace. I wouldn't recommend this, especially as you don't appear to have any decoupling caps at the IC pins. I think this is likely to end up being problematic. If it were my board I would try and use polygon fills top and bottom to get your Vcc and GND connected around the board as much as possible. Obviously with a 2 layer board you're going to end up cutting up any polygon fills with all the other traces running around but I would give this a try to see how it works. Secondly, it's obviously auto routed and there are several places where the nets just go really close to things when there is bags of room for them to have a little more clearance. Examples would be the traces running very close to X2 and the ones around J1 but there are plenty of examples all over the board. I'd recommend you have a go at manual routing on the board, you'll pretty much always get a much nicer result. Best Regards, Rachael

Amega328p-au shorted pins ?

Top Replies