First SMT PCB - ready for board house?

Discussion in 'The Projects Forum' started by bkochis, Sep 8, 2010.

  1. bkochis

    Thread Starter New Member

    Aug 5, 2010
    19
    2
    I have created this SMT PCB board and am looking for a critique.

    DRC is complaining about clearances. The complaints are mostly about the msop-8 packages for the LM3478 and LM3488 chips.
    Am I doing something wrong here?

    This board is to power a HP printer from a car battery. It outputs 16v @ 0.5a and 32v@ 0.9a. I used .016 traces for the Vcc and GND connections.
    Are the traces large enough?

    I will be trying to create this board at home using the laser printer/clothes iron method. If it does not come out correct, I will be sending it out for someone else to create. I am concerned about my ability to create pads close enough for the msop-8 package. :eek:

    I have attached a .zip file with the Eagle schematic, board and Gerber files.

    Thank you for your time.
     
  2. gootee

    Senior Member

    Apr 24, 2007
    447
    50
    If you go to 4pcb.com and submit your Gerber files to their free design-checking unility, it should automatically email you PDF files of the layers, and also descriptions of any manufacturability problems with the design, as well as pricing (try upping the quantities and see how little the total price changes!). I don't have Eagle. But I can view PDF files.
     
  3. marshallf3

    Well-Known Member

    Jul 26, 2010
    2,358
    201
    If using the toner transfer method you're in for some fun as they keep changing the paper everyone tends to recommend as being the best. A couple of years back Staples Basic Glossy photo paper was supposed to be the best, now it won't work worth a darn and has plastic on the back too so it messes up your iron.

    Don't foget to double check everything - remember that an SMD board usually needs to be a mirror image to use the toner transfer method with.

    Invest in a small stainless ruler that will measure in 100th of an inch or 10th of a mm so you can check that too - printers aren't always anywhere near as accurate as you might think.

    All depends on your program too. DIPTrace has printed quite a few boards for me that were absolutely dead on as far as size went but that's only if you print out of the program, if you save the file as a .jpg or bitmap you may as well forget it.

    I've got the best results using a very white (100 or better) common laser paper using a Savin printer with their factory toner. It has a pretty high melting point so you have to use the iron method, a common laminator won't work no matter how many times you pass the board through.

    Don't get in a hurry wanting to pull the paper off either, let it soak for hours or even overnight.

    And as mentioned above 4pcb's Free DFM service can be handy in spotting traces that are too close for comfort. I've been known to alter the parameters for through hold boards but SMDs are just too picky when it comes to soldering so I'd stick with their recommended spacing.
     
  4. kubeek

    AAC Fanatic!

    Sep 20, 2005
    4,670
    804
    The schematic is extremely illegible and ugly, you need to use the power symbols, but that is not the point of this thread.

    1) traces are way too thin and could end up broken and not working, use the default 0.016 as a minimum, unless you need to pass between legs of a component
    2) if you don´t plan to use plated holes, you won´t be able to solder the top connections of the power jack X2
    3) for hand soldering use at least 0805 resistors, better 1206 to make the soldering easier, also it makes for simple passing of traces between the legs
    4) watch out for the clearances of vias near M2 and U$6, seems a bit too close
    5) USE the DRC tool! Set the parameters that your fab house is capable of and test the board
    6) power needs to go first through the smoothing caps and then to the rest of the circuit, simply paralelling or connecing them somewhere won´t do. The same for the CBYP caps, they are supposed to be AS CLOSE AS POSSIBLE to the part they are meant for, sure not across the PSU terminals
    7) I am pretty sure M1 and M2 have multiple pins connected to drain and source, use them all and use thick traces for high current paths (i mean really thick)
    8) the board is HUGE for the number of components and complexity, i suggest ripping everything up and doing it again after placing the components closer
    9) use ground plane on both sides, conencted to ground (make a filled polygon around the whole board, set the right clearance and rename it to GND)

    And back to the schematic, you should make the circuit easily understandable first, placing the components at the right places to show where the parts should actually be. Then start with the board, making traces as short as possible. The board sholud really be packed with components, this way you are wasting very costly space.
     
    bkochis likes this.
  5. kubeek

    AAC Fanatic!

    Sep 20, 2005
    4,670
    804
    I just read your original post more carefully, for iron transfer, even 0.016 is too thin.
    I think the MSOP package just isn´t doable, try to find it in some other package.
    0.6 and 0.9A need at least 100mil traces, probably even more, and I don´t think the transistors will handle the dissipation, also from the schematic it looks like they have ground connected to both drain and source.
    Also the both parts of the PSU on the board should be symmetrical or same, and for sure not interconnected like that.
     
    bkochis likes this.
  6. gootee

    Senior Member

    Apr 24, 2007
    447
    50
    Actually, you should be able to do .01-inch traces with toner transfer. But you might have to get the method working quite well first, for that.
     
  7. marshallf3

    Well-Known Member

    Jul 26, 2010
    2,358
    201
    I try not to go below 0.03", I'll even sneak in a jumper if necessary to avoid getting too thin of a trace or one that's too close in proximity. And yes, 1206/1210 size components make things easier.
     
  8. bkochis

    Thread Starter New Member

    Aug 5, 2010
    19
    2
    Thanks for the info guys.

    Huh, I only received one email that a response to my post had been created.

    Anyway, Kubeek, thanks for the report card on the circuit! I will go back and look at the design produced by webench at National.com. I thought I was 'packing it in' as far as parts placement goes. The board is only 2x3". :D I will do as you suggest and start from scratch with this.

    As fas as the laser/iron method goes, gootee, you are the first article that I found that actually mentions tolerances achieved.

    I am baking the transfers in a toaster oven at 450°F for 12-14 minutes between two 1/4" aluminum plates with about 3 pounds of steel on top. Transparencies gave the quickest transfer but had shrinkage problems if I over baked them. Laserjet photo papers are showing some promise.

    Thanks all,
     
  9. marshallf3

    Well-Known Member

    Jul 26, 2010
    2,358
    201
    It's hit and miss to find the right paper, often inkjet paper (which can be used in a laser printer) works better than some laser paper.

    I was really excited with the resolution and toner coverage I got with that glossy inkjet photo paper in a laser but alas, too much plastic in the paper made separation almost impossible. Some people swear by using the glossy newspaper inserts you find in the Sunday paper, others with glossy paged magazines and have for years. Since the ink used in these is virtually always soy based it doesn't interfere.

    It's all a combination of the paper, the printer and the specific toner involved. Eventually you'll hit on a combination that will allow some really good results.
     
    bkochis likes this.
  10. bkochis

    Thread Starter New Member

    Aug 5, 2010
    19
    2
    Sorry I have been offline fighting a virus and did not want to take any chances spreading it.

    Anyway, here is the second attempt. I used http://www.desmith.net/NMdS/Electronics/TraceWidth.html to set the widths and clearance values.

    I was able to etch a test board with traces of the correct size for the msop8 package using the laser/iron/muriatic acid method.

    Any critique of the board is appreciated.

    Thanks in advance.
     
  11. t06afre

    AAC Fanatic!

    May 11, 2009
    5,939
    1,222
Loading...