zeke 693 Posted October 3, 2011 Share Posted October 3, 2011 Doh... I was going to copy that part into my lib and change it so it has that pad broken out in the schematic... Forgot. Will get that So a SMD XT2 is preferable to TH?... I've got a ton of TH... :\ Could do it though. R5/C4 & R4/C3 I used the same layout as on the LP (trace may be a little diff)... I've got no idea how to route those USB lines other than how I did? :-\ (I struggle with the basics of EE...) I can add the ESD's no problem... R10, C13, C14 = Followed from F5529 Experimenters Board, didn't fully research... R8 and R9 are in the datasheet If you have a ton of TH crystals then your choice makes sense. The guy you sell this board to may not though. The only gotcha with a TH crystal is that you can't let the body of the crystal touch the ground plane you've poured under it. If it does then it probably is also touching the tracks coming from the crystal pins and that shorts out the crystal. That's why TH crystals had insulator pads on them in ancient days. The USB tracks should make the straightest line between the connector and the chip as reasonably possible. Make sure the tracks are 0.010" wide. Make sure they have a 0.010" space between them. That's it. Any components that have to attach to the USB tracks should do so at a 90' angle so that the track path isn't disturbed. It is also preferable to minimize their length, if possible. I haven't consulted the design files for TI's 5529 board so I don't understand their design selections. The 27 ohm resistors are there to minimize the transient responses that occur on the USB lines. They limit the current spikes but they also lower the maximum speed on that transmission line. I guess it all depends upon the MCU and what it expects. For comparison, the FTDI chips want 0 to 10 ohms there. There's no need to worry about your EE skills. You are demonstrating good EE skills with your work. Just because I'm buffing your layout doesn't mean it's a bad design. I'm sure the design will work. I'm just offering a contrasting opinion for you to compare against. It's like two artists talking about a work of art - a matter of taste and opinion for the most part. Again, GOOD JOB! And I mean it! :thumbup: gordon, tripwire and SugarAddict 3 Quote Link to post Share on other sites
gwdeveloper 275 Posted October 3, 2011 Share Posted October 3, 2011 I would prefer SMD crystals as well. The HC49 that Zeke recommended works fine or for slightly smaller, I like the MC-306 package that epson uses. http://www.mouser.com/Search/ProductDetail.aspx?R=MC-306_32.7680K-A0%3aROHSvirtualkey99990000virtualkey732-MC30632.7680KA0R TI has a design note for 32KHz oscillators too. Not sure if you've seen it. http://www.ti.com/lit/an/slaa322b/slaa322b.pdf It's what I'm using for designing my F2274 board. EDIT: BTW, no pressure on ya but I'm really excited about this board. Definitely put me down for 4 of them. Quote Link to post Share on other sites
SugarAddict 227 Posted October 4, 2011 Author Share Posted October 4, 2011 If you have a ton of TH crystals then your choice makes sense. The guy you sell this board to may not though. My plan was to solder the whole thing before hand. I've already got 10 F5529's and will order all the other components as soon as I've got a solid board headed for the fab. I can always leave these unsoldered and put out what values I have and can solder. The only gotcha with a TH crystal is that you can't let the body of the crystal touch the ground plane you've poured under it. If it does then it probably is also touching the tracks coming from the crystal pins and that shorts out the crystal. That's why TH crystals had insulator pads on them in ancient days. Nice... I can easily put them in the air a bit... The USB tracks should make the straightest line between the connector and the chip as reasonably possible. Make sure the tracks are 0.010" wide. Make sure they have a 0.010" space between them. That's it. Any components that have to attach to the USB tracks should do so at a 90' angle so that the track path isn't disturbed. It is also preferable to minimize their length, if possible. I'll give that a shot, as best I can I haven't consulted the design files for TI's 5529 board so I don't understand their design selections. The 27 ohm resistors are there to minimize the transient responses that occur on the USB lines. They limit the current spikes but they also lower the maximum speed on that transmission line. I guess it all depends upon the MCU and what it expects. For comparison, the FTDI chips want 0 to 10 ohms there. Dunno, TI does things odd... I felt that I should use the same values and the 2 caps and resistor since there must be a reason for them. There's no need to worry about your EE skills. You are demonstrating good EE skills with your work. Just because I'm buffing your layout doesn't mean it's a bad design. I'm sure the design will work. I'm just offering a contrasting opinion for you to compare against. It's like two artists talking about a work of art - a matter of taste and opinion for the most part. That was in reference to not knowing the USB stuff... I can go on and on about what I have zero clue about so I just sum it up that I don't know most of the basics, because I really don't... lol. And the buffing is good, it's what I asked for Thanks! I'll work on that and post it again soon'ish. One other Q I had was about the Vcc line I've got going around the board, the spots that connect to it are 90 Quote Link to post Share on other sites
SugarAddict 227 Posted October 4, 2011 Author Share Posted October 4, 2011 Updated... Is it ok that I did that the way I did with the crossover? Quote Link to post Share on other sites
zeke 693 Posted October 4, 2011 Share Posted October 4, 2011 Updated... Is it ok that I did that the way I did with the crossover?Schematic Board I'm not sure what the crossover is specifically. One other Q I had was about the Vcc line I've got going around the board, the spots that connect to it are 90 SugarAddict 1 Quote Link to post Share on other sites
SugarAddict 227 Posted October 5, 2011 Author Share Posted October 5, 2011 Where the DM goes under the DP, Had to criss-cross them... Kinda sucks they have them on the chip that way. Quote Link to post Share on other sites
SugarAddict 227 Posted October 7, 2011 Author Share Posted October 7, 2011 Ok, I did go ahead and put HC49/U on there and will order a few 32MHz, 24MHz, 16MHz for this... I will probably get some standard green boards later and have the through hole on those... Depending on how well this works out... Pictures: [attachment=2]F5529-Dev-Final-3.png[/attachment] Quote Link to post Share on other sites
ike 53 Posted October 7, 2011 Share Posted October 7, 2011 Why don't you use R8 to cross other trace? Quote Link to post Share on other sites
zeke 693 Posted October 7, 2011 Share Posted October 7, 2011 Crossing the trace is not a good thing. Blows the transmission line characteristics all to "H.E. double hockey sticks". It will result in slow USB speeds and other unintended consequences. Re-route the USB traces off the backside of their pads and they will re-orient themselves properly to the USB connector. You'll have to move the PUR trace to the frontside of its pad and then, using vias, route it over to the switch. You'll then be able to keep the VBUS trace on the topside. Just re-route it off the frontside of its pad as well. bluehash and SugarAddict 2 Quote Link to post Share on other sites
SugarAddict 227 Posted October 8, 2011 Author Share Posted October 8, 2011 One of those suggestions that makes you go "Why didn't I think of that?!?!?" lol DONE! RobG 1 Quote Link to post Share on other sites
zeke 693 Posted October 8, 2011 Share Posted October 8, 2011 Just click that little thumb sign for me :mrgreen: BTW, just to be picky, it looks like R8 & R9 are about 0.040" apart. The kinks in the USB N&P tracks cause an impedance discontinuity. To avoid that, you could skooch R8 and R9 closer together so that their sides line up with the track edges. It will then look like a straight line. Good work! :thumbup: SugarAddict 1 Quote Link to post Share on other sites
SugarAddict 227 Posted October 8, 2011 Author Share Posted October 8, 2011 Though I'm leary about the two being so close... Done and ordered. Will post to this thread again when it's here and I've got one soldered up Quote Link to post Share on other sites
PentiumPC 119 Posted October 8, 2011 Share Posted October 8, 2011 Though I'm leary about the two being so close... Done and ordered. Will post to this thread again when it's here and I've got one soldered up A newbie suggestion , will be nice if some pins can breakout to take the booster packs.. Quote Link to post Share on other sites
bluehash 1,581 Posted October 9, 2011 Share Posted October 9, 2011 uh-oh... Don't let him repent placing his order PPC. Glad to know your order went through SA. Quote Link to post Share on other sites
RobG 1,892 Posted October 9, 2011 Share Posted October 9, 2011 That's what revisions are for bluehash There will always be another board after v1, because there will always be something to improve, so no repents. Quote Link to post Share on other sites
Recommended Posts
Join the conversation
You can post now and register later. If you have an account, sign in now to post with your account.