From schematic to board layout - Help & hints needed - Page 2 - diyAudio
Go Back   Home > Forums > Design & Build > Construction Tips

Construction Tips Construction techniques and tips

Please consider donating to help us continue to serve you.

Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving
Reply
 
Thread Tools Search this Thread
Old 22nd July 2011, 11:46 AM   #11
marce is offline marce  United Kingdom
diyAudio Member
 
Join Date: Jun 2007
Location: Blackburn, Lancs
Possibly tweek the QFP footprint, the PDF is for an IPC-7351 (Industry Standard) footprint.
Also look at some of the routes going into pads, 90 deg into the pad is prefferable, then add a 45 degree bend, otherwise you can create acid traps.
Attached Files
File Type: pdf QFP32.pdf (43.3 KB, 26 views)
  Reply With Quote
Old 26th July 2011, 02:10 PM   #12
diyAudio Member
 
Join Date: Mar 2011
Location: Jyväskylä
Thanks for your input! I have tried to implement all your suggestions in this revision. Does it look any better? Ground and VCC traces are wider (25 mils vs. 10 mils). All the grounded pins now have dedicated vias, the crystal has ground pour as guarding and the capacitors on other side. I also tried to remove all the non 90-degree entries from the pads to avoid acid traps. The schematics are attached (the resistors have capacitor symbols because I didn't have a 1206-sized resistor part at my library, lazy me, so don't mind that). C9 and C4 are the decoupling caps.

All input is highly appreciated, and thanks again to marce!

Click the image to open in full size.
Attached Files
File Type: pdf Rev_B_sch.pdf (10.7 KB, 27 views)
  Reply With Quote
Old 29th July 2011, 11:11 AM   #13
marce is offline marce  United Kingdom
diyAudio Member
 
Join Date: Jun 2007
Location: Blackburn, Lancs
Again beef up power tracks, and swap the position of X1 with C6, C10 and R3, the caps and rsitor between the IC and the crystal, what you have now is a stub with the caps and resistors hanging on the end. In a rush at the moment, but I will find an example of a crystal over the weekend.
  Reply With Quote
Old 29th July 2011, 11:47 AM   #14
diyAudio Member
 
Join Date: Mar 2011
Location: Jyväskylä
Ah, true, I forgot to swap the capacitors on the other side and just changed the R3. I'll make the power traces even larger (is there a width when it's not worth going any wider?).
  Reply With Quote
Old 30th July 2011, 07:51 AM   #15
marce is offline marce  United Kingdom
diyAudio Member
 
Join Date: Jun 2007
Location: Blackburn, Lancs
Download this toolkit, it has loads of useful information, nearly all PCB designers I know have a copy on their desktop for instant use.
PCB Via Current | PCB Trace Width | Differential Pair Calculator | PCB Impedance

The file 1-xtal.png is an example of a crystal, using a 5x7 package instead of the SMD HC49 package.
The file 1-lay.png is a snapshot of a layout showing some power tracks and signal tracks to give you an idea of the relative sizes.
Most boards I do are multlayer, so always have power and ground planes. On a double dided board I always use the bottom layer (non component side) for the ground plane as this gives the best contigous unbroken ground plane, and put vias down to this plane for ground connections. I would also copper pour ground on to the top layer once I have finished routing the board.
Attached Images
File Type: png 1-xtal.png (31.9 KB, 35 views)
File Type: png 1-lay.png (52.9 KB, 39 views)
  Reply With Quote
Old 30th July 2011, 08:02 AM   #16
marce is offline marce  United Kingdom
diyAudio Member
 
Join Date: Jun 2007
Location: Blackburn, Lancs
Some more comments, sorry.
These are refinments, what you have is OK and I have seen some proffesionaly designed boards that are less attractive, but these are the icing on the cake.
Turn C7 and C5 180 degrees, you can avoid the track between the pads, best to do this where possible on samll MLCC caps.
Align the pins of C13, R6 & C14 and run a track straight between the pins.
Rotate R10 90 deg and avoid the split in the route.
Rotate C1 and reposition slightly, again to avoid route between pins.
REMOVE Thermal Relief from all vias, it is not needed.
Rotate R7 and put in line with connector, straight routes again.
Sorry for being pedantic, but these little changes will clear the layout up.
Have Fun
Marc
  Reply With Quote

Reply


Hide this!Advertise here!
Thread Tools Search this Thread
Search this Thread:

Advanced Search

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are Off
Refbacks are Off


Similar Threads
Thread Thread Starter Forum Replies Last Post
Preamp with limiter schematic, need some hints petrol vendor Instruments and Amps 0 15th August 2008 05:48 PM
Look over this amp board layout please. MJL21193 Solid State 10 22nd November 2007 01:40 AM
Amplifier Layout - Help & advice needed andrew_whitham Tubes / Valves 5 8th May 2007 08:49 PM
Grounding & board Layout questions Valvomaniac Tubes / Valves 1 26th April 2007 03:56 AM
Denon PMA 770 - Schematic & PCB layout - Anyone got one? GeorgeBoles Solid State 1 29th September 2004 11:50 PM


New To Site? Need Help?

All times are GMT. The time now is 06:59 PM.


vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2014 DragonByte Technologies Ltd.
Copyright ©1999-2014 diyAudio

Content Relevant URLs by vBSEO 3.3.2