OS MTM PCB Creation

Discussion in 'DIY Speakers and Subwoofers' started by ScottS, Jan 9, 2017.

  1. #1 ScottS, Jan 9, 2017
    Last edited: Jan 10, 2017
    Hi everyone,

    While I waited for the OS MTM kit to get in stock, I spent my time designing a PCB for the crossover. I'm getting ready to pull the trigger to get it produced and am wondering if any one can provide feedback. I used KiCad to do the design.

    You may review my files (and screenshots!) here: OSMTM-PCB

    My biggest question is this: I'd like to use banana binding posts on the board as I feel it's plain easier to make the connections. (OK, also, I wasn't entirely sure which of the screw terminal footprints to use and which ones to buy...) but now I'm unsure if this particular post will do the trick on my board. The size is correct, but will it actually make the connection onto the board, or will it get signal from both the top and bottom layers?

    Other than that, does anyone else have any feedback?

    Once I get boards produced that I'm happy with, I'll tag a release on git and generate downloadable files that then anyone can come along and send to their PCB fab shop to get produced.

    Thanks for looking!
     
  2. First off. I believe the schematics are not supposed to be posted online, unless you got permission from DIYSG. Same goes with making the PCB design available to the public. I could be wrong though so best check with Erich.

    Regarding your layout:
    1. Traces seem a bit thin, what width are they?
    2. You don't need 4 sets of holes to zip tie the inductors, one would do.
    3. I personally would not use a banana plug inside the speaker box because it may come loose in the future. Just solder it, save your money.
    4. Are you using a ground plane? Doesn't hurt but it looks like it is preventing you from doing a single sided board which will be cheaper.
     
  3. I did ask Erich if he'd be interested in including these boards as options with his kits (thinking like some kits offer just the bezel, others the full knock down cabinet as an add-on) and he suggested just posting to the forums. Of course, I actually need to get one built and verify that it works... And FWIW, the schematics are posted on the creator's website.

    1. You're absolutely right. I did the math for what trace width I needed for 4.5A and then mistakenly plugged in the value for the external, not internal traces. Good catch. They're not ~5mm and much larger.
    2. Removed, mostly.
    3. Those are also changed to screw terminals.
    4. I am, yes. Just seemed to be the default, so I rolled with it.

    New board layout, front, back.

    Thanks for the feedback, and great catch with the trace widths.
     
  4. External traces should have been fine. Are you using a SW for calculating trace widths?

    Can't tell for sure whether the pads are small, what is the diameter? You may want also Increase the gap between your ground plane and your traces.

    The ground plane would be hard to solder to. If you decide to keep it, add thermal reliefs to make soldering easier.
     
  5. Yes, I used this calculator. Figured sqrt(120W / 6 Ohms) ~= 4.5 was the max current needed to be supported. In retrospect I probably neglected to put in a valid length, as that seems to impact the results greatly.

    The holes above 0.762mm because the specs for the resistors and capacitors said that their leads were 0.5mm +/- 5%. Another person has suggested increasing these drill holes to 1.5mm for the resistors and caps, then 1.6mm for the inductor, so I've increased those.

    There are thermal reliefs in place but they are 0.5mm and were the default values. Do you have a suggestion for a reasonable value, or a resource I can run some calcs?
     
  6. Trace length should have no impact on temp rise. Are you using 1oz copper?

    Yeah, 0.762mm would be really small for the component leads to go through. I have used 1.4mm with good results for both the capacitors, resistors and inductors (18AWG).

    As for themals, I use a 10mil gap with the thermals covering less than 50% of that gap. But this is dependent on a lot of things including your fab house capabilities and solderability of the board. Looks like your defaults are fine.

    What's your pad size for the components?
     
  7. Not sure what to think. Just found this...

    http://www.pcb-3d.com/knowledge-base/pth-dimensions

    Minimum Hole Size = Maximum Lead Diameter + 0.25mm (for Level A of IPC-2222)
    Minimum Hole Size = 0.525mm + 0.25mm = 0.775mm

    The pad diameter for that hole would be 1.475.

    Pad Diameter = Minimum Hole Size + 0.1mm + 0.60mm (for Level A of IPC-2221)
     
    ja00 likes this.
  8. Those numbers would be the minimum, and that is if the parts are actually 0.525mm max. I have one of the resistors and measured it to be 0.72mm. The inductors also come tinned, so it is hard to say what the final diameter is on those.
     
  9. Thanks! You're not the first one to say that the leads are measuring closer to 0.7 vs the quoted 0.5mm. Because of that, I've increased the drill holes to 1.5mm with a hole size of 3mm. There are now some more substantial thermal reliefs to help with the soldering. It was also suggested to add some cable relief holes for the screw terminals.

    You can checkout the new layout here: https://github.com/SirScott/osmtm-pcb/tree/feature/100x100
     
  10. #10 ja00, Jan 13, 2017
    Last edited: Jan 13, 2017
    The picture you posted does not look complete, is that correct?

    It looks like you overdid the thermals. The defaults you had would probably have worked. Can you post a picture of that?

    Also I recommend you place components that electrically connect together closer to minimize the trace length. For example, L2 and C3 are in parallel, are best placed next to each other. I kind of understand why you did it the way you did though - to minimize board size (cost) if I am not mistaken...

    One other thing, check your vias.
    1. They are passing the same current as your traces.
    2. Depending on your board house - min diameter for the thickness of the board to ensure your via walls don't end up being incomplete. Add more vias if you need more current handling

    Oh, and add some separation between non electrically connected traces to prevent accidental short - gap is dependent on who will be doing the assembly. Soldermask should help with but best have that extra clearance.
     
  11. Yes, it should be. What did you feel was missing? (I don't have 3D models for the inductors so those do not show up, but the footprint is reserved.)

    It looks like you overdid the thermals. The defaults you had would probably have worked. Can you post a picture of that?

    That's exactly right. If the overall dimensions can be < 100mm x 100mm, the cost of production is $1/board, a significant savings. I started by creating a square at that size, putting the mounting holes, then placing the inductors at opposite ends. The leftover space forced my hand with respect to component layout.

    Good call on the vias. I'm not sure how to do those calculations, so will be hitting up google!

    My components have shown up and the initial board should be showing up in the next day or two. (And my initial measuring of the components confirms your 0.77mm lead diameter - way off from the PE quoted 0.5mm!)

    I'll get things tested on the bench shortly, then make tweaks as appropriate.

    Thanks for the help!
     
  12. You're welcome.

    So then I assume the pins marked as RED is connected to the top plane and the BLACK on the bottom plane?
     
  13. Wish I'd seen this thread sooner. I designed and manufactured a crossover PCB for the OS MTMs last year.
    [​IMG]
     
  14. Inside, with a matte white baffle. I designed them to fit through the cutouts, if need be. Finished size of 85mm X 140mm.
    [​IMG]
     
  15. I designed them using 7mm tracks, gold plating, and accommodation for up to 14 guage hook up wire (I used 16ga. for this pair).

    [​IMG]
     

Share This Page