PCB Track Width and pad size

Discussion in 'The Projects Forum' started by bumclouds, May 20, 2009.

  1. bumclouds

    Thread Starter Active Member

    May 18, 2008
    82
    0
    Hey guys,

    I'm very new to making PCB's. I have to make one for one of my uni projects, and I have NO idea what size to make the pads, and what thickness the tracks should be.

    I also don't know how to make those "feet" that I've seen people put in the corner of PCB's, and I dont know what size you should make the holes for those..

    I'll give you a schematic of mine, to show you the currents and voltages..

    [​IMG]

    So far I've done a track width of 3mm for everything. How is that?
     
  2. beenthere

    Retired Moderator

    Apr 20, 2004
    15,815
    282
    Low currents don't need a lot of track width. 3mm is probably 3 or 4 times what you actually need. I would be comfortable with .024" leads, which are about .61mm. Make the pads a comfortable size - that is something you determine by experience and how good you are drilling the holes.

    The largest concern you have is in keeping tracks spaced apart so the B+ doesn't go places it shouldn't.

    You know this project should be done on a chassis with the components underneath run point-to-point on terminal strips.
     
  3. bumclouds

    Thread Starter Active Member

    May 18, 2008
    82
    0

    What does that mean? :confused:
     
  4. beenthere

    Retired Moderator

    Apr 20, 2004
    15,815
    282
    Last edited: May 20, 2009
  5. bumclouds

    Thread Starter Active Member

    May 18, 2008
    82
    0
    So what's the advantage of doing the old fashioned way as opposed to PCB?
     
  6. beenthere

    Retired Moderator

    Apr 20, 2004
    15,815
    282
    That was not serious advice - the tubes are old-fashioned, so I was suggesting the project be done using an old-fashioned method.
     
  7. Darren Holdstock

    Active Member

    Feb 10, 2009
    262
    11
    It is claimed by many guitarists that the old tag-strip method made a nicer sounding amp than mounting the valve circuitry on a PCB. Usually some vague voodoo about the tag-strip and PCB materials are given by way of explanation, but this is never backed up by solid theory or experimental results. The paper/resin construction of tag-strip is slightly leaky compared to FR4 PCB, but not enough here to make a difference I think. If there indeed is any difference between tag-strip and PCB sound, it will be because of the better mechanical coupling with the tag-strip method, as the valve base is bolted directly to the metal chassis, whereas with a PCB the valve base is soldered to the board itself. This means that the tag-strip valve will be more subject to acoustic vibration from the loudspeaker, which given the microphonic nature of valves makes for a "warmer" sound. The valve on the PCB will have lower microphonic effects because of less efficient acoustic coupling, and these will also be coloured by the acoustic resonant characterstics of the PCB itself.

    Nice uni project, BTW, hope you get extra marks for style.
     
  8. bumclouds

    Thread Starter Active Member

    May 18, 2008
    82
    0
    Thanks ^_^. I think I will go the with the PCB option. My lecturer said he'd prefer a PCB. I'm also a bit of a noob with making PCB's, so this will give me a good chance to learn.

    I'm having a tinnyy little problem with making my PCB in protel. I have little Vcc and Gnd ports in the schmetic editor, and when I choose to update the PCB from schematic, it won't work.. and those error messages are all in relation to what resistors or caps are connected to Vcc or Gnd.

    :( hm..
     
  9. bumclouds

    Thread Starter Active Member

    May 18, 2008
    82
    0
    I got really mad at protel and did all the routing by hand.

    Here is the print preview of what I've done.. How is it? Does anything stand out as being totally wrong?

    [​IMG]
     
  10. Wendy

    Moderator

    Mar 24, 2008
    20,766
    2,536
    Why is the trace on C1 so long. Looks like you could simplify some there.

    Also, leave holes in the pads, it will aid in drilling later.
     
  11. AlexR

    Well-Known Member

    Jan 16, 2008
    735
    54
    As others have said the sig input area of the board needs reworking, also some of the track/pin spacings look a shade close considering that Vcc (that should be B+ by the way) is 200 volt. And lastly did you forget the heater wiring or are you going to run it in hook-up wire rather than PCB tracks?
     
  12. bumclouds

    Thread Starter Active Member

    May 18, 2008
    82
    0
    Okay, i'll try shortening some of the traces as much as I can.

    I'll change Vcc to B+. So if the voltage is as big as 200V I should try to keep the clearance bigger you're saying?

    Regarding the pad sizes..

    What size holes should I put in the pads? Say I make the smaller pads 1mm in Radius, and the hole 0.5mm in radius, leaving a ring of width 0.5mm, is that good enough? Is there some rule to do with pad sizes and hole sizes I can go by?

    Thanks for all the help guys ^_^.
     
  13. Wendy

    Moderator

    Mar 24, 2008
    20,766
    2,536
    Figure just a shade smaller than the drill bit you will use.
     
  14. Darren Holdstock

    Active Member

    Feb 10, 2009
    262
    11
    That's a bit small. The local heat cycling from the valve will stress the solder joints, so bigger pads would be favourite. For through-hole Rs and Cs I'd go no smaller than 2 mm diameter, preferably 2.5 mm. If you're hand-etching and drilling the PCB then I've found through experiment that a 0.7 mm hole on the pad artwork works well in centring drill bits from 0.8 to 3 mm diameter. Normally the holes for 1/4 W Rs and small Cs are 0.8 mm.

    Check the valve base datasheet for recommended pad and hole sizes. They may recommend a few cooling holes in the PCB around the valve too.

    Ditto the other comments on track clearance.
     
  15. AlexR

    Well-Known Member

    Jan 16, 2008
    735
    54
    The general standard hole size for low wattage resistors and capacitors is 0.8mm. Board manufacturers generally state that the pad size should be at least .5mm larger than the drill size but in practice if you are drilling the board by hand I would not go below 1.65mm (65mil) pads.

    Your circuit is low current so track width is not that important, if you keep them in the .4mm - .7mm (15mil - 25mil) range it should be fine.

    I think the thing bothering us about your input routing is the double tracks going to pin 2 of the valve, why not just join Rin and C1 directly and have only one track going to the valve pin?
     
  16. bumclouds

    Thread Starter Active Member

    May 18, 2008
    82
    0
    Okay, I've redone the PCB.

    The R and C pads are 2.0mm Pads, with 0.7mm holes (why won't the holes show up on the print preview?).

    I actually forgot a couple of things which I've now put in..

    Is it better? ..Or have I made it worse..

    [​IMG]
     
    Last edited: May 21, 2009
  17. Darren Holdstock

    Active Member

    Feb 10, 2009
    262
    11
    I get the same issue with Protel. For some reason the tracks ends that connect to a pad obscure the hole when printing. It's a rather annoying bug, and the only workaround I know is to segment the track within the pad and reduce the width of the track stub to something very small (or maybe zero, I forget). It's a massive pain, and if anyone knows of a better workaround I'd be grateful to hear it.

    Don't forget your heater supplies, BTW. You might need some means to support the PCB too - I like hex pillars for convenience. A 7 mm pad with a 3 mm hole will support a 3 mm-thread post.

    The PCB is getting there; could be tidied up somewhat though. C1 looks as though it will foul the valve base, the vsource track could do with being moved away from Vbb, and you can route vout1 without going through the valve pins by taking it through R4, R5 and R7 (shuffle R4 and flip R5). Might as well flip R2 and C4 while you're at it.

    You may get a couple of extra project points by making the PCB look nice, which is not just aesthetics as a decent layout invariably performs better and is more reliable. Some simple guidlines that work well are things like:
    - Changes in track angle are always 45 degrees
    - Track-to-track connection angles are never less than 90 degrees
    - Clearances between adjacent copper nets should be as large as possible (e.g. run a track track through a resistor mid-way between the legs, not close to one pad and further away from the other).

    A well-designed PCB will invariably look elegant, which is no coincidence. I do appreciate that bumclouds is at the placement stage of the layout, and things always do look a bit rough until it's tidied up. But the tidying is easy (if a little repetitive), the real hump is getting the placement right, which bc has done a good job of.
     
  18. bumclouds

    Thread Starter Active Member

    May 18, 2008
    82
    0
    Thanks so much for taking the time to give me all that advice.!! I appreciate it so much, as I'm really new to this.

    I've gotta go to work now, but as soon as I get back from work I'll update my PCB with all the things you suggested, and I'll post another image.

    I also might make my PCB bigger, as I just realised this Print Preview seems to scaled to about 2:1, and when I drew it 1:1 on paper, it looked to be about the size of the palm of my hand.. So I'll make the board bigger. I think it would look nicer that way.

    And the heaters.. How do I wire up the heaters and what do I do? My lecturer never mentioned anything about them!

    PS: this is what the data sheet says about the heaters:
    [​IMG]


    Is one of the columns DC and the other one AC?
     
    Last edited: May 22, 2009
  19. Wendy

    Moderator

    Mar 24, 2008
    20,766
    2,536
    The early tubes heaters used AC, 6.3V, which is why it is a standard for transformers. Many cases the transformers had more voltage, so they put the filaments in series so they would drop about the right voltage across each one. Of course, if one filament burned out all the tubes stopped working (and their filaments went dark).

    I don't know for sure, but I don't think it makes any difference if the voltage going to the filament is AC or DC, as long as the voltage is right (RMS rules in this case).

    BTW, put your name on that board. It is worth signing your work, and it may be used by other websites for the amplifier, in which case it is nice to get credit where credit is due.
     
  20. bertus

    Administrator

    Apr 5, 2008
    15,648
    2,346
    Hello,

    With the E-series the voltage is "constant" at 6.3 or 2 X 6.3 Volts.
    With the P-series the current is "constant" at 0.3 Ampere. These are usualy put in series.

    For tube data take a look at this page:
    http://www.nj7p.org/Tube4.php?index=1

    Greetings,
    Bertus
     
Loading...