Jump to content
43oh

F5529 Breakout Dev Board (Now with pics!)


Recommended Posts

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:

Link to post
Share on other sites
  • Replies 99
  • Created
  • Last Reply

Top Posters In This Topic

Top Posters In This Topic

Popular Posts

Got the boards today from Seeed... couldn't help but solder at least one up... and I'm sad... the USB is failing (Unknown device / malfunctioning device) but programming it via a LP with SBW works fin

So this is a work in progress... A fair bit of it is a copy off of TI's 5529 Experimenters Board because it's the basics required for operation... some of it just looked sane as well. Simple RC filte

And now that parts finally showed up (yay for china ordering...) here's two pics of a fully pop'd one. I will be sending 3 of these to the store for BH at some time in the future... might send him th

Posted Images

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.

Link to post
Share on other sites

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... :D

 

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 :D

 

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 :D 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

Link to post
Share on other sites

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.

Link to post
Share on other sites

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:

Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.


×
×
  • Create New...