Soldering suggestions for a DO-214AB package diode?

Hi Andrew,

It is a SMC 2-Lead footprint and it would be easy and inexpensive to have an adapter board made by someone like OSH Park (less than $2 with shipping).  Are you familiar with any of the PCB design tools?  If not, this would be an easy project to learn on.

Frank

Hi Andrew,

It is a SMC 2-Lead footprint and it would be easy and inexpensive to have an adapter board made by someone like OSH Park (less than $2 with shipping).  Are you familiar with any of the PCB design tools?  If not, this would be an easy project to learn on.

Frank

I'll look into that - I've used JLCPCB recently and they've been very good.  I do have KiCad downloaded but not used it yet - I could certainly give it a go.

Thanks

Andrew

I use KiCad and this would be a good starter project for it.  Out of curiosity I checked to see if it had the SMC footprint built in and it does.  In fact, it has a hand solder version which I had a look at.  There is a via through the footprint to a pad on the other side in their hand solder version which is interesting.  It would be easy to solder.  I encourage you to try building it yourself but let us know if you would like suggestions or feedback.

I’m going to start on that today!

Thanks everyone.

Hi Frank,

just following up on this earlier conversation.  I set up about working out how Kicad works and creating a PCB.  I tried with the SMC footprint, and Kicad has three in its library:

1 - what looks to be a 'textbook' sized footprint

2 - what looks to be 'textbook' sized, but rotated by 90deg

3 - what looks to be 'textbook' sized, rotated by 90deg with through holes in them (the one you show above.)

With the rotated pads, the actual component would span the space between the pads and I'm assuming that the pads are larger in order to allow a soldering iron to get to them?  Is there a danger that the solder flow pulls the component off the other pad and more into the centre of the pad being soldered (is that question clear??) - basically, in order to span the pad gap, the component must be soldered at the edges of the pads, not the middle.

Generically, would it be easier to solder these components with a hole in the pad?  Are there any tips/gotchas to be aware of when designing boards with SMD components?

I actually took a first project of mine - a very, very, very simple switched regulated power supply - and built the schematic, PCB and Gerber files for it.  A 'test' with JLCPCB indicated it seems fine and I think I amazed myself at how quickly I seemed to pick it up!  However, the devil is likely in the detail: if it's not too cheeky would you be able to take a look and see if I've done anything crazy, or could do something better?  I'm not asking to see whether my circuit is any good - it works well for what I needed it for, but I know I can improve it (and when I built it the switches and LEDs were off-board) - it's really just a sanity check on my Kicad schematic/pcb as I'm going to actually create something in anger now.  I didn't need to create any new footprints or add any special libraries so it should be ok with version 5.1.

Kicad zip on my OneDrive: https://1drv.ms/u/s!AkgMkSdwBcLBgite8nuAUTe4douy

Gerber zip on my One Drive: https://1drv.ms/u/s!AkgMkSdwBcLBgiqqITiwd0kldSl3

Thanks,

Andrew

Hi Andrew,

Both Doug and Shabaz are more experienced than me but here are my thoughts....

 

With the rotated pads, the actual component would span the space between the pads and I'm assuming that the pads are larger in order to allow a soldering iron to get to them?  Is there a danger that the solder flow pulls the component off the other pad and more into the centre of the pad being soldered (is that question clear??) - basically, in order to span the pad gap, the component must be soldered at the edges of the pads, not the middle.

 

Generically, would it be easier to solder these components with a hole in the pad?  Are there any tips/gotchas to be aware of when designing boards with SMD components?

 

In an automated process the solder is spread across a stencil onto the pad for a SMD part.  The recommended size of the opening on the stencil is normally on the datasheet for the part.  In manual soldering of SMD a stencil can be used but it is also possible to just dab some solder paste on, especially with larger parts like this one.  Or, rosin core solder can be used but small diameter is recommended.  I normally use 0.3 mm.   There is always a space between the pads and ideally it would be covered with solder resist which helps prevent solder from bridging.  Some board houses allow closer spacing than others and still get solder resist, check their fabrication guidelines.  It might try to pull the part away during hand soldering but if it does just hold it down with tweezers or something.  You would not use the oversize pads for automated soldering.

The stop mask determines how much area is exposed next to the pad. KiCad has a large default mask expansion and I always reset it.  See this description of recommendations for KiCad at OSH Park:  https://docs.oshpark.com/design-tools/kicad/

If the 3D render is turned on in the KiCad viewer the placement of the part can be viewed.  For example here is the part I posted earlier.

The part is centered between the pins with lots of room to get a soldering iron in.  Solder should ideally form a concave fill on the side of the pin on the SMD part and will wick under the part as well.   I treated the through hole like a large via and it would allow excess solder to wick to the bottom and might provide for a bit of heat transfer.   I am not familiar with doing 2 lead SMD parts this way though.  Typically I would provide for a somewhat longer pad just to make sure the iron can get in.  Many of the SMD parts in the KiCad library have a hand solder version that does just that so have a look at those.  This one is excessively large if all that is needed is getting the iron in.

 

 

I actually took a first project of mine - a very, very, very simple switched regulated power supply - and built the schematic, PCB and Gerber files for it.  A 'test' with JLCPCB indicated it seems fine and I think I amazed myself at how quickly I seemed to pick it up!  However, the devil is likely in the detail: if it's not too cheeky would you be able to take a look and see if I've done anything crazy, or could do something better?  I'm not asking to see whether my circuit is any good - it works well for what I needed it for, but I know I can improve it (and when I built it the switches and LEDs were off-board) - it's really just a sanity check on my Kicad schematic/pcb as I'm going to actually create something in anger now.  I didn't need to create any new footprints or add any special libraries so it should be ok with version 5.1.

 

Kudos for designing this yourself in a real design tool and posting.  My first thought is to make sure the traces on the PCB will carry the current as I am not sure what they are in your design.  There are online calculators as well as a built-in calculator in KiCad.  PCB design is a personal thing with lots of personal preferences and I won't outline mine.  Dave Jones has some videos and there are others as well.  But here are some quick observations:

There is a trace going nowhere inside the yellow highlight so delete that.  I would move the traces with the red highlight away from the pads even though they might meet the DRC.  You have plenty of real estate to do it.  Other than that, if the schematic is correct there is a good chance the PCB will turn out OK. Always label the parts on the silk screen, mark polarity where needed, give it a name, and date.

Good work and good luck

Frank

Thanks for your input Frank.

I did recreate that part and looked at it in 3D, and what you say makes sense to me.  I’ve bought a ‘practice’ kit to have a go and looked for .3mm solder, but blimey it’s expensive in leaded version!  I’ll give it a go with my .6mm and see how I get on  

I thought I’d picked up all the spare tracks; I found the track-laying the most awkward part of the tool, plus they don’t move with the parts.  I also now notice the sharp-angled joins in some areas.  I set the parameters for the board based on JCLPCB requirements first; the actual current carrying requirement of the tracks is max 1A and I calculated that at 0.15mm - I used the Kicad default which, IIRC, is 0.25mm (not in front of the ‘pootah at the moment).  Anyway, I take your point and thanks for the pointers - I’ll take a look at the Oshpark info.

Really appreciate your time,

thanks,

Andrew

Consider beefing up the traces....  Most prototype boards are made with 1 oz/ft2 copper weight.  Here is a screen shot from this site:  https://www.4pcb.com/trace-width-calculator.html

Assuming the design current is 1 A and the trace is 5 cm long the resulting 0.3 mm trace width results in a fair voltage drop and power loss on the external layer.  Or, for an even simpler approach, this site recommends 1 mm / A:  Minimum Trace Width ~ PCB Design Tech Guide.  There are plenty more varying guidelines out there.

So, back to KiCad.  The default width may be OK for your use but there is no shortage of space on your board and an amp is a fair amount of current.  I use the default settings on KiCad for signals but bump up trace width a bit for power if there is room.  Look at how thick the pale yellow trace on the SMD part I drew up.  Undoubtable overkill on my part but keep it in mind....

I'm sure I used that calculator and got .15mm!  I'll dig deeper into this, and Kicad, thanks for the heads up. 

Thanks

Andrew

Hi Andrew,

I've not used KiCAD so I can't point to the specifics, but there will be a design rule check (DRC) tool in KiCAD, and running that will pick up things like traces too close to holes. It possibly might not pick up that trace that Frank highlighted in yellow, since that may not be violating any of its rules, even though it is not needed.

There's a bit of extra resistance with the thin traces, so there would be a voltage drop if high current is passing, even if the traces can handle the slight rise in temperature, so you might prefer to thicken up some of them. That is impressive that you've done the schematic entry and PCB design with KiCAD as a first attempt.. I think it would electrically function.

Regarding the diode land pattern/footprint, as Frank says, there will be a recommendation in the datasheet, so that can be a start. For nearly all SMD parts, I find the default recommendation to be acceptable for hand-soldering too, even though the datasheet land pattern is normally for an automated process (e.g. reflow or wave). As Frank says, optionally you could increase the size of the pad outward, to make it a bit easier if the pads don't already extend much beyond the component physical dimensions in the datasheet. Sometimes I may extend by 0.3mm or so, for certain components which have an overhang (e.g. large surface mount inductors with an outer ferrite shield that goes beyond the land pattern). For that diode package, that isn't the case, so the datasheet land pattern should be fine.

I'm not sure why there are holes in the land pattern, I'm wondering if they are for optionally soldering a through-hole diode instead, i.e. the land pattern is dual-purpose maybe.

Normally holes in pads are not used unless they are filled (i.e. commercial PCBs) since solder will drip through otherwise, but for home prototyping sometimes they are necessary (in which case I'll try to use the smallest hole possible). For a SMD diode breakout board, the holes shouldn't be needed in the pad I think, unless I'm missing something.

Thanks Shabaz.  I realise now I didn’t change the default copper thickness used in the calculator, which is 2oz, so I ended up with half the value that I should have.

The pads in the data sheet are about half the width of those used above, enough area for the two tabs under the component which would make it difficult for hand soldering - I guess paste and a hot-air gun would be needed.  This conversation has given me a bit of insight in how to decide on, or adjust, footprints for SMD parts.  And to ensure I double check my calculations   It does seem sometimes that there are so many things to get wrong!!

Thanks

Andrew