Forum Update - Announcement about May 10th, 2018 update and your password.

Propeller PCB Layout Template and First Attempt

24

Comments

  • Peter JakackiPeter Jakacki Posts: 7,467
    edited June 13 Vote Up0Vote Down
    I haven't seen your board yet but you can always take a screenshot or save a png or pdf of it that you can post so that anyone can see at first glance.

    Tracks can be narrow and carry high currents, it comes back down to how long they are and how thick is the copper which is normally 1oz because all this relates to resistance which relates to heat and indirectly any heat sinking effects etc. But your standard 0.1" header pins should be ok for around 1A depending upon the contact material used on both ends although I have pushed these but once again it becomes a matter of resistance and heat. Prolonged heat will cause the spring in the connector to lose its spring and therefore the pressure it applies to lower the contact resistance. Short bursts are ok but once the contacts are heat damaged they will only get worse.

    So I might run 20 or 30 mil wide tracks for power but usually I do copper pours for ground and maybe for power if necessary. If in doubt use 2 pins for power and 2 for ground but at the moment I'm just guessing because I haven't seen it yet.

    Tachyon Forth - compact, fast, forthwright and interactive
    useforthlogo-s.png
    --->CLICK THE LOGO for more links<---
    Latest binary V5.4 includes EASYFILE +++++ Tachyon Forth News Blog
    P2 SHORTFORM DATASHEET +++++ TAQOZ documentation
    Brisbane, Australia
  • I haven't seen your board yet but you can always take a screenshot or save a png or pdf of it that you can post so that anyone can see at first glance.

    Tracks can be narrow and carry high currents, it comes back down to how long they are and how thick is the copper which is normally 1oz because all this relates to resistance which relates to heat and indirectly any heat sinking effects etc. But your standard 0.1" header pins should be ok for around 1A depending upon the contact material used on both ends although I have pushed these but once again it becomes a matter of resistance and heat. Prolonged heat will cause the spring in the connector to lose its spring and therefore the pressure it applies to lower the contact resistance. Short bursts are ok but once the contacts are heat damaged they will only get worse.

    So I might run 20 or 30 mil wide tracks for power but usually I do copper pours for ground and maybe for power if necessary. If in doubt use 2 pins for power and 2 for ground but at the moment I'm just guessing because I haven't seen it yet.
    I'm afraid I don't have a board layout yet. I'm struggling to try to fit this into a 3.8x2.5 rectangle. The autoplacer in DipTrace produces a larger board so I'll have to tweak it by hand.

  • David Betz wrote: »
    I haven't seen your board yet but you can always take a screenshot or save a png or pdf of it that you can post so that anyone can see at first glance.

    Tracks can be narrow and carry high currents, it comes back down to how long they are and how thick is the copper which is normally 1oz because all this relates to resistance which relates to heat and indirectly any heat sinking effects etc. But your standard 0.1" header pins should be ok for around 1A depending upon the contact material used on both ends although I have pushed these but once again it becomes a matter of resistance and heat. Prolonged heat will cause the spring in the connector to lose its spring and therefore the pressure it applies to lower the contact resistance. Short bursts are ok but once the contacts are heat damaged they will only get worse.

    So I might run 20 or 30 mil wide tracks for power but usually I do copper pours for ground and maybe for power if necessary. If in doubt use 2 pins for power and 2 for ground but at the moment I'm just guessing because I haven't seen it yet.
    I'm afraid I don't have a board layout yet. I'm struggling to try to fit this into a 3.8x2.5 rectangle. The autoplacer in DipTrace produces a larger board so I'll have to tweak it by hand.

    Place your components manually and if you can view the ratsnest connections then do it as you can move your components around and work out the best placement so that most of the connections should need almost no special routing. While paying attention to clearances etc don't worry overly much about them if you manually route until later as it starts to shape up.




    Tachyon Forth - compact, fast, forthwright and interactive
    useforthlogo-s.png
    --->CLICK THE LOGO for more links<---
    Latest binary V5.4 includes EASYFILE +++++ Tachyon Forth News Blog
    P2 SHORTFORM DATASHEET +++++ TAQOZ documentation
    Brisbane, Australia
  • One thing I've wondered about is how to deal with the voltage regulators. The footprints I found for them seem to for mounting them vertically but I'd like them to lie flat on the PCB. Do I just need to manually leave enough space for that or is there a way to modify the footprint with DipTrace to allow for flat mounting?
  • You can do either. I have seen designs where a vertical footprint is used and then a mounting hole is placed appropriately to support horizontal mounting as an option. Making a dedicated footprint is better as it allows you to expose some copper for the heatsink to make contact with in cases you are worried about heat dissipation. I will look to see if I have any DipTrace footprints for a horizontal TO-220.
  • How does this look? I still have the regulators mounted vertically but I think I found a footprint that will let me mount them horizontally. I just have to remember where I saw it! :smile:
    965 x 655 - 296K
  • T ChapT Chap Posts: 3,780
    edited June 13 Vote Up0Vote Down
    You can just as easily use an SMT regulator. It’s very easy to hand solder or use air. You can find a rework station for 100$ if you don’t have one. I use this 500ma part on most of my prop boards. The point being that you can make this board with all SMT parts and it’s not a lot of work to hand solder the parts. But if you want to put the regulator as SMT only to start then you would find out how easy it is for future reference. Granted a stencil and solder paste would make it easier.

    LP38691DTX-3.3/NOPBCT-ND. At Digi


  • T Chap wrote: »
    You can just as easily use an SMT regulator. It’s very easy to hand solder or use air. You can find a rework station for 100$ if you don’t have one. I use this 500ma part on most of my prop boards. The point being that you can make this board with all SMT parts and it’s not a lot of work to hand solder the parts. But if you want to put the regulator as SMT only to start then you would find out how easy it is for future reference. Granted a stencil and solder paste would make it easier.

    LP38691DTX-3.3/NOPBCT-ND. At Digi

    That looks pretty easy to solder. Thanks!

  • Ugh. I have a PCB layout I'd like to try. I designed it with DipTrace and wanted to have it fabricated by ExpressPCB but it seems ExpressPCB can only accept boards designed with their own ExpressPCB software. I don't see a way to import a DipTrace file into ExpressPCB to place the order. Does anyone know of a way to do this?
  • PublisonPublison Posts: 10,192
    edited June 13 Vote Up0Vote Down
    David, you can order directly out of Diptrace to BayArea Circuits. They are a good US based circuit house. (File>Order PCB. I think JonnyMac has used them).
    Infernal Machine
  • Publison wrote: »
    David, you can order directly out of Diptrace to BayArea Circuits. They are a good US based circuit house. (File>Order PCB. I think JonnyMac has used them).
    I just noticed that and placed my order after making a minor change in my layout. Now we'll see whether it works! :-)
  • Did you do a final copper pour for the ground at least? A good ground is everything and I saw plenty of places where an easy point to point track could have made it better. Be aware that while this board may work, that once you start drawing a bit more current with a few more cogs and switching more loads that the circuit may seem to glitch, crash or worse still, you fry your Prop due to unbalanced ground currents. Worse yet again, it works, well most of the time except for those mysterious glitches.

    Tachyon Forth - compact, fast, forthwright and interactive
    useforthlogo-s.png
    --->CLICK THE LOGO for more links<---
    Latest binary V5.4 includes EASYFILE +++++ Tachyon Forth News Blog
    P2 SHORTFORM DATASHEET +++++ TAQOZ documentation
    Brisbane, Australia
  • David Betz wrote: »
    Publison wrote: »
    David, you can order directly out of Diptrace to BayArea Circuits. They are a good US based circuit house. (File>Order PCB. I think JonnyMac has used them).
    I just noticed that and placed my order after making a minor change in my layout. Now we'll see whether it works! :-)

    Cool beans! Post pic when they come in.

    I just ordered a home PCB kit that JonnyMac has been using to try a couple of prototype boards.

    https://pcbfx.com/main_site/pages/start_here/overview.html
    Infernal Machine
  • Did you do a final copper pour for the ground at least? A good ground is everything and I saw plenty of places where an easy point to point track could have made it better. Be aware that while this board may work, that once you start drawing a bit more current with a few more cogs and switching more loads that the circuit may seem to glitch, crash or worse still, you fry your Prop due to unbalanced ground currents. Worse yet again, it works, well most of the time except for those mysterious glitches.
    Yes, I added a copper pour for ground on both sides of the board. I assume that is likely to help with the issues you mention. The next time I do this I think I'll just lay out the board by hand. It doesn't seem like it would be that hard. I notice that the auto-router generated a lot of via's. Not sure if that is a problem.
  • Oh ok. Yes, those autorouters can very pretty dumb. Take this connection to R4, it's a classic.
    vias.png
    240 x 162 - 29K

    Tachyon Forth - compact, fast, forthwright and interactive
    useforthlogo-s.png
    --->CLICK THE LOGO for more links<---
    Latest binary V5.4 includes EASYFILE +++++ Tachyon Forth News Blog
    P2 SHORTFORM DATASHEET +++++ TAQOZ documentation
    Brisbane, Australia
  • Oh ok. Yes, those autorouters can very pretty dumb. Take this connection to R4, it's a classic.
    vias.png
    I'm sure I probably confused it by moving things around manually and then running the auto-router again... repeatedly.
  • Yep, that can happen when you move a trace that has a via that was previously required. DipTrace will not automatically strip "newly-unnecessary" vias during a re-route.
  • Yep, that can happen when you move a trace that has a via that was previously required. DipTrace will not automatically strip "newly-unnecessary" vias during a re-route.
    If I had noticed that I guess I could have manually fixed it. It might be easier though to just manually layout the next PCB that I attempt. I'm just hoping this one will work!

  • David,

    Use thicker traces for power (and ground, too, if don't have a ground plane). 30 mils should be adequate; 50, if you have room. Also, if you're using a ground plane, be sure to heat-relieve your pads, or you'll have a bugger of a time soldering them.

    -Phil
    “Perfection is achieved not when there is nothing more to add, but when there is nothing left to take away. -Antoine de Saint-Exupery
  • Cluso99Cluso99 Posts: 13,770
    edited June 14 Vote Up0Vote Down
    Hi David,
    Sorry I am late to the party as I have been quite busy. Anyhow, here are a few suggestions for next time...
    Note that none of what you have done is incorrect.

    Schematic
    Unless you are using a polarised capacitor, as in electrolytic or tantalum, it is usual to use a symbol with two straight bars. FYI the curved is as you used, the ground/negative terminal.
    GND connections are usually represented by a vertical line going to a flat horizontal or triangle. See my P8XBlade2 thread. I prefer a different 3V3connection.
    Try and keep your connectors consistent. eg keep pin 1 at the top if possible.
    On larger ICs like the Prop, it's common to have the +PWR connections at the top of the IC and GND at the bottom. Not so common for smaller ICs such as the 8-pin. Here it is often easier to keep the pinouts as per the IC. ie pin 1 top left and clockwise from there, 4 each side.
    For the Prop, it's nicer to have p0-P15 on one side, and P16-P31 on the other. ie keep the 8 pin groups together.

    PCB Layout
    It would have been much better to use larger traces for power and ground, and/or power and ground pours.
    Your 3V3 ad GND rails are important. These should be placed first and by the most direct route. Note how your 3V3 rail snakes around the board to the prop pins. It would also be best to have the most direct route between the 3V3 on each side of the prop. Same for GND. This ensures the prop pins are at the same voltage. Note in your circuit, C5 is not across pins 9 & 12 where it is supposed to be.
    Try and keep your parts closest to where they are used. eg U3 & U4 are at the opposite end of the prop from where they are being driven, and for U3,closer to the J4 & J5.
    Since you have a 9x1 header with P0-6 plus 3V3 and GND, it may have been better to have P0-7 connected using a 10x1 header - ie make it more future proof???
    Again, the power rail to the header coming via the prop power pins is not good. If there is a power drain/slump caused by the header, it will be seen by the prop. If it came direct from the regulator, C4 & C5 would help protect the prop.
    The power & Gnd rails for U8, U3 & U4 would normally be run in parallel tracks under the chips from top to bottom of the pcb. Caps between the chips and at top and bottom end would complete the rails. I note that U3 is 5V and not 3V3 so there is a problem doing this properly.
    People often criticise a pcb when the connectors do not all fall on a 0.1" grid. I note your J5 & J2 (&U1) are off grid compared to J3,4,6,7 & J1.
    BTW your choice of an SMT xtal is unusual wrt all other thru' hole parts.

    Crystal routing
    FWIW we try to keep tracks as close/short as possible to the chip, and if possible keep other traces away from these, particularly clocking signals. Often a ground ring is placed around the xtal too. It is always best to check on special considerations in the chip datasheets as there are often specific requirements. The P1 is quite general in this regard, but other ICs can be very demanding!

    Having said all this, for your first design, you have done a good job. And, the prop is quite forgiving too.
    I hope this helps :)


  • David,
    My TriBlade was the only DIP40 Prop design I did (as I never built my Six blade).
    Here is the schematic and pcb layout. Sorry, most of the underside is not visible here. My design is archived and packed aways as we move next week.
    It may give you some tips.
    bluemagic.biz/clusodocs/sixbladeprop_schematic.pdf
    forums.parallax.com/discussion/download/59055/Cluso_TriBladeProp_375.bmp

    and my TriBlade thread
    forums.parallax.com/discussion/110563/triblade-prop-pcb-uses-3-propeller-ics-for-a-single-board-computer-sbc/p2
  • Cluso99 wrote: »
    Hi David,
    Sorry I am late to the party as I have been quite busy. Anyhow, here are a few suggestions for next time...
    Note that none of what you have done is incorrect.

    Schematic
    Unless you are using a polarised capacitor, as in electrolytic or tantalum, it is usual to use a symbol with two straight bars. FYI the curved is as you used, the ground/negative terminal.
    GND connections are usually represented by a vertical line going to a flat horizontal or triangle. See my P8XBlade2 thread. I prefer a different 3V3connection.
    Try and keep your connectors consistent. eg keep pin 1 at the top if possible.
    On larger ICs like the Prop, it's common to have the +PWR connections at the top of the IC and GND at the bottom. Not so common for smaller ICs such as the 8-pin. Here it is often easier to keep the pinouts as per the IC. ie pin 1 top left and clockwise from there, 4 each side.
    For the Prop, it's nicer to have p0-P15 on one side, and P16-P31 on the other. ie keep the 8 pin groups together.

    PCB Layout
    It would have been much better to use larger traces for power and ground, and/or power and ground pours.
    Your 3V3 ad GND rails are important. These should be placed first and by the most direct route. Note how your 3V3 rail snakes around the board to the prop pins. It would also be best to have the most direct route between the 3V3 on each side of the prop. Same for GND. This ensures the prop pins are at the same voltage. Note in your circuit, C5 is not across pins 9 & 12 where it is supposed to be.
    Try and keep your parts closest to where they are used. eg U3 & U4 are at the opposite end of the prop from where they are being driven, and for U3,closer to the J4 & J5.
    Since you have a 9x1 header with P0-6 plus 3V3 and GND, it may have been better to have P0-7 connected using a 10x1 header - ie make it more future proof???
    Again, the power rail to the header coming via the prop power pins is not good. If there is a power drain/slump caused by the header, it will be seen by the prop. If it came direct from the regulator, C4 & C5 would help protect the prop.
    The power & Gnd rails for U8, U3 & U4 would normally be run in parallel tracks under the chips from top to bottom of the pcb. Caps between the chips and at top and bottom end would complete the rails. I note that U3 is 5V and not 3V3 so there is a problem doing this properly.
    People often criticise a pcb when the connectors do not all fall on a 0.1" grid. I note your J5 & J2 (&U1) are off grid compared to J3,4,6,7 & J1.
    BTW your choice of an SMT xtal is unusual wrt all other thru' hole parts.

    Crystal routing
    FWIW we try to keep tracks as close/short as possible to the chip, and if possible keep other traces away from these, particularly clocking signals. Often a ground ring is placed around the xtal too. It is always best to check on special considerations in the chip datasheets as there are often specific requirements. The P1 is quite general in this regard, but other ICs can be very demanding!

    Having said all this, for your first design, you have done a good job. And, the prop is quite forgiving too.
    I hope this helps :)

    Wow! Thanks for all of the advice. I think my biggest problem may have been using the auto-router. I won't do that next time. Then I can place things where I want them. Also, I didn't intentionally use an SMT crystal. I found it difficult to figure out what footprints to use and made a mistake with that one. I hope I can somehow find a way to solder one of my through-hole crystals in that position when the board arrives.
  • If in doubt, don't leave it out. Use dual footprints, one for the through hole, one for the surface mount, and even overlay them if possible.

    Tachyon Forth - compact, fast, forthwright and interactive
    useforthlogo-s.png
    --->CLICK THE LOGO for more links<---
    Latest binary V5.4 includes EASYFILE +++++ Tachyon Forth News Blog
    P2 SHORTFORM DATASHEET +++++ TAQOZ documentation
    Brisbane, Australia
  • David Betz wrote: »
    jmg wrote: »
    David Betz wrote: »
    Here is my first attempt at a schematic. This board contains a basic Propeller circuit plus two outputs to drive WS2812 LED chains. It also contains a rotary encoder with an RGB LED and push button switch and a connector for a 16x2 parallel LCD display. Does anyone see any red flags before I try to lay out a PCB? One thing I'm really not sure of is how to get the bypass caps positioned correctly on the PCB. I just have them attached to the power and ground nets in the schematic.

    Those LT1085/LT1085 are not cheap as regulators go - do you need a lot of current / voltage ?

    I like the look of the new ST LDL1117 series.
    Those are like an improved LM317, with fixed outputs, and much lower Iq and low drop out.
    Low cost in a SOT223, and with high PSRR, good to 18V, so not as high V or W as the LT1086, but fine for most 9~12V plug power sources.
    The low dropout means you can power this from 5V
    The Propeller Platform schematic I was working from used LD1085 and LD1086. I couldn't find those in the libraries but did find the "LT" parts. I think they have the same pinout so I can always substitute other regulators. I might be interested in fairly high current to allow driving lots of WS2812 LEDs although I'm also providing a way to supply 5V from an external power supply as well.

    Don't get caught trying to drive many 100's of milliamps from a 5V linear regulator just because the regulator specs says it can. The more current it handles times the more voltage it is "dropping" is the power it must dissipate which in such a small package and lack of heatsinking can be a source of smoke and woe. So 12V to 5V at a measly 100ma = 7x0.1 = 700mW which is still very hot for small regulators. Use an external 5V or use a switching regulator. Personally I switch down to 5V and use small SOT89 packs or even SOT23 for my 3.3V. There are plenty of cheap 3-pin "7805" style switcher modules available these days, they run nice and cool and being switchers they will draw less current from say 12V then they supply at 5V etc. Rough rule is say 85% efficiency so 5V @ 500ma = 2.5W divided by 12V and by 0.85 is approx 245ma @12V.
    Are you saying to use a 7805 for the 5v supply and a LD1117 for 3.3v? Can I just use one in place of the LT1086 regulator I was planning on using possibly with different caps? I think the pinouts and circuits are the same. I don't think the LD1117 is available in a TO-220 package.

  • jmgjmg Posts: 11,674
    David Betz wrote: »
    Are you saying to use a 7805 for the 5v supply and a LD1117 for 3.3v?
    If you plan on 9~24V, Peter was meaning all of the words of "7805" style switcher modules ie parts that are actually complete modules, than can (hopefully) fit into a TO-220 PCB

    VXO7805-500 CUI Inc. DC DC CONVERTER 5V 2.5W Min 6.5V or 7V Max 36V or 31V Vo 5V or -5V 500mA or 300mA 2.5W
    Through Hole 3-SIP Module
    VXO7805-1000 CUI Inc. DC DC CONVERTER 5V 5W Linear Regulator Replacement 1 8V 36V or 27V 5V or -5V
    When you are starting from a much higher voltage, at reasonable currents, these are much lower power loss.
    David Betz wrote: »
    Can I just use one in place of the LT1086 regulator I was planning on using possibly with different caps? I think the pinouts and circuits are the same.
    Are you sure ? The '7805' generic pinout has GND in the centre pin.

  • David Betz wrote: »
    How does this look? I still have the regulators mounted vertically but I think I found a footprint that will let me mount them horizontally. I just have to remember where I saw it! :smile:

    Here's a single sided board I did using Diptrace. It has a switch mode power supply feeding 3.3 and 5.0 volt linear voltage regulators, a battery backed real time clock, two 12 bit ADCs feed by instrumentation amplifiers configured for unity gain, 5 optically isolated 28 VDC inputs, and 6 optically isolated 28 VDC solenoid drivers. The board controlled a 7.5 HP 3 phase electric motor driving a 3000 PSI hydraulic pump and associated flow control valves to run a hydraulic grapple used in logging. The board could have been made much smaller but it just had to fit in an existing enclosure that was quite large so lots of room and wide traces were possible. By placing the EEPROM as I did and using the resisters for the SPI lines as jumpers I was able to keep the board single sided. It's the first board I ever designed.

    Sandy
    1024 x 768 - 223K
    Infantryman's Axiom; Always cheat, always win.
  • David Betz wrote: »
    How does this look? I still have the regulators mounted vertically but I think I found a footprint that will let me mount them horizontally. I just have to remember where I saw it! :smile:

    Here's a single sided board I did using Diptrace. It has a switch mode power supply feeding 3.3 and 5.0 volt linear voltage regulators, a battery backed real time clock, two 12 bit ADCs feed by instrumentation amplifiers configured for unity gain, 5 optically isolated 28 VDC inputs, and 6 optically isolated 28 VDC solenoid drivers. The board controlled a 7.5 HP 3 phase electric motor driving a 3000 PSI hydraulic pump and associated flow control valves to run a hydraulic grapple used in logging. The board could have been made much smaller but it just had to fit in an existing enclosure that was quite large so lots of room and wide traces were possible. By placing the EEPROM as I did and using the resisters for the SPI lines as jumpers I was able to keep the board single sided. It's the first board I ever designed.

    Sandy
    Looks a lot better than my first board and mine is simpler. My PCBs arrive today. I hope I can get them to work with all of the mistakes I made. In the meantime I'm trying to learn how to use KiCad for the next one.

  • David BetzDavid Betz Posts: 12,202
    edited June 22 Vote Up0Vote Down
    I got my PCBs and now I'm wondering if I should even try assembling them. I see now what people were talking about with respect to the power connections. There are very long narrow traces and the bypass caps are not located in the right positions. The ground connections aren't really a problem because I did a ground copper pour on both the top and bottom. Is the board likely to work at all or should I save the components and order more PCBs with the power problems fixed?
  • Can you post a pic of the top and bottom
  • T ChapT Chap Posts: 3,780
    edited June 22 Vote Up0Vote Down
    You could always try it out and see if it works for your application. You can also run some Wires as needed and you can also hand solder bypass caps. It’s not unusual on your first couple of boards to need to do some hacking and patching.
Sign In or Register to comment.