SMPS Design E25/13/7, coil crafting questions and pointers!

[minimer]

Hello Everyone!

I'm new here so forgive me if I didn't find the answer to my questions in my brief search of the posts! I am embarking on my first isolated AC to DC SMPS power supply design. I'v built several power systems over the years but flyback systems have always kind of scared me lots of places to go wrong. 

To the point then, I cant find a transformer that fits the requirements any where online or even in any of the SMPS circuits I'v harvested. However I can find a coil former for winding my own. I have taken a few of these buggers (flybacks) apart and I get the basic idea of construction, but there are some things I am not clear about.

First the coil former I have selected! The third attachment is its data sheet.
http://www.newark.com/epcos/b66208b1110t1/coil-former-e25-13-7-valox-420se0/dp/79T4675?in_merch=Popular%20Products 

The first attachment is a graphical representation of how the transformer should be constructed. The second attachment is an image of the reference design circuit if any one is curious.

My questions are as follows!
1. How important is the right hand rule in a flyback, will Faraday's integral law bite me in the arse if I don't observe it!
2. What kind of tape should I use, and what kind of copper foil if any! I am considering kapton is that acceptable?
3. Is there anything special I should consider about terminating the wingdings???
4. Do I need to wrap all the layers individually and connect them at the terminals? If they are all connected in series any way, can I wrap the first primary and possibly the second primary all at once instead of terminating them and layering the secondary between them. 
5. The primary and AUX coils are all enamelled that makes sense.. but the secondary is labeled Triso? Can any one tell me what that means?
6. Is there anything I should know other than what I'v asked!

Thank you ahead of time for insight!

[minimer]

AcHmed99!

Thank you very much for your reply, Kapton is a brand name for polyimide silicone adhesive tape! I love the stuff I call is space duct tape, I think its better than Mylar tape but perhaps its not advantageous with its dielectric properties or maybe its too expensive who knows why they don't use it commercially for this...

Any way, What do you mean by starting at the drain end? I am familiar with triple insulation didn't know it was called Triso learn something new every day. I also have seen this interesting type of gap tape used in some of the higher quality transformers I have taken apart, typically its used to fill in the gap left behind where a coil terminates before it has filled to the end of the bobbin do you know where I can find any of that stuff of should I just use tape!

Thank you for the part recommendation, I started with the E25 because I had a prebuilt library in my CAD for it. But then I realized I could take advantage of how and where I terminate the wingdings to save space on my PCB, so I will be building my own libraries for this any way because the pinouts will be different mine as well use a better part!

Now about the schematic this was automatically generated by an online application at NXP's website, I agree R1, and R2 don't seem right I also don't like how the input is protected. I would prefer standard Y caps in series and X cap across L and N and I will change it because I don't trust their solution. I'm going to spend some time smacking that schematic in the face and reading the TEA1733 datasheet. Hopefully in a few  hours from now ill post my own version of the schematic.

[megajocke]

**You have at least one error in your schematic you have R1 nad R2 connected to your AUX output. Those are bleeder caps for your EMI filter cap they go between L and N.

What's the problem there? The resistors are doing double duty as bleeders for the EMI filter cap while providing the startup supply to the control IC.

[minimer]

megajocke,

I suppose the problem is I have an irrational predisposition to not understanding this circuit. I thought the voltage divider between R4 and R7 provided the startup power, but after your reply and reading over the data sheet your spot on. R4 and R7 are just for voltage sensing. Just for my sake I investigated the demo boards NXP provides for the TEA1733 and they all do exactly the same. I considered adding to Y caps from L and N respectively to the AC ground. But I have not seen this in any of the demo board designs they all use a single Y to couple the grounds. After my research I don't see anything else to change in the circuit! I guess time to layout the board!

[minimer]

If anyone is interested,

Here is my schematic and board layout! Designed for continuous operation 50 watts 36 volts! If any one would like the eagle files or gerber files reply or let me know! I also have an up to date BOM for digikey! Total cost is about $36 USD not including PCB. If you skip out on all the nice caps and other proper components iv selected its about $24 USD. This cost assumes you wind your own flyback!

[planet12]

Couple of comments:

1. Your auxiliary supply is being brought out on the low-voltage side of the transformer (pins 6/10). This is not going to allow the requisite clearance and creepage distances between the high and low voltage circuits, and indeed does not with the current layout. As-is this would fail safety certification... now you don't necessarily need safety standard certification for what you're doing, but you'll make your supply safer by aiming to meet them anyway.

2. You could probably reduce the loop area of the fast-changing-current paths, eg. the C1-T1-Q1-R6 loop. Get traces as short as possible, and do things like running return paths on the other side of the board directly under the trace taking current in the other direction. Minimising the loop area here will reduce radiated EMI.

HTH

[minimer]

Planet12,

Thank you for your thoughts! I have an interesting trade off here.. Size vs proper component and power isolation. I have found it makes more sense to change the size of the board a little, most of the readily available enclosures are more rectangular.
I wanted this to be the size of a laptop charger give or take but I'm skeptical. I might need to increase in size even more to ensure I have all the AC ground on one side, isolated on the other. To route this board its kind of "all over the shop".

But a fun practice none the less. I route all my boards this size and complexity manually start to finish.. I find when I build the schematic while routing I get more out of my design.  I'm anxious to hear what you think about the new design!

And for fun here is a fat version of the board v1.2. All the low voltage components are on their proper side of the optocoupler! Much better isolation.

[planet12]

Definitely improved in relation to the transformer, but you've snatched defeat from the jaws of victory in a couple of other places - most notably directly underneath the optocoupler, due to routing traces from primary and secondary sides within what looks to be about 0.024" of each other.

You basically want to have a clear space at least as wide as between your optocoupler's primary and secondary side pins. I've drawn a translucent yellow line on your v1.2 layout image showing what I mean.

This line should be about 6mm wide, and pass through the centre lines of your transformer and optocoupler. Use polygons on the top and bottom restrict layers in Eagle, and let nothing violate them. If the closest any primary and secondary conductors come is at the opticoupler, that would be ideal.

The other thing I noticed is that you're taking the ground feed for the primary control circuitry from the transformer pin, rather than directly from the negative leg of the main reservoir capacitor. The trace between the reservoir cap and the transformer pin is going to be carrying moderately large but also fast-changing currents, and it's going to cause ground bounce / ground noise in your control circuitry. You want to think about a "star earth" but with emphasis on separating the high current and high di/dt returns from the control returns.

Are you just using the IRF540 for the layout, and are actually using a different MOSFET? I ask as the VDS of that is only 100V.

[minimer]

Thank you again!

I really think I'm getting closer now. No I have beefed up most the components a tad. A few of the surface mount caps might could use a through hole replacement namely the 4.7 uF cap on the start up voltage/bleeder C11. I found an 0603 reasonably priced for the job but I'm skeptical. Here is a BOM and a new design!

[planet12]

Good catch AcHmed99 - I suspect the RCD clamp components might turn into blue smoke very rapidly!

http://www.cde.com/tech/design.pdf has a section "Component selection and layout" regarding snubbers/clamps I'd recommend you read.

You're definitely heading in the right direction now with the safety clearances - I can see at a glance some places you can widen the isolation with only moving a couple of tracks, but it's vastly improved over earlier revisions.

EDIT: typos.

[Neilm]

There are some very good app notes out there. I found this one very useful in understanding exactly what was going on with a snubber. Very helpful when looking at the waveforms to see if it was performing correctly.

Neil

[minimer]

Thank you Everyone,

I have improved the snubber circuit components 3 watt low inductance metal film resistor and high quality high voltage mica capacitor together they added 10 percent to the total cost but im sure it will be worth it! Hopefully they can handle the job. I'm going to trust the design's recommended values for both of them as they can be tweaked later when the circuit is actually performing. Here is the newest version of the board there is still one trace that gets close to the keepout and some of the component pads it is the driver trace for the MOSFET. Its turning out t o be the hardest trace to rout in every design so I might omit it and use a wire jumper. I realize that is opening the drive circuitry to all sorts of interference but so is a tiny trace snaking its way all along the board. 

Please tell me what you think I hope soon it can be off to the board house with this one!

[planet12]

Important first: just noticed you have a direct earth-to-neutral connection on the board. This may not be a good idea, and may even be illegal to connect to the mains. Check the earthing system for the country this will be used in.

Second: how wide is your creepage zone between primary and secondary? It doesn't look like 6mm (0.24") to me (actual requirements differ per country and max input voltage).

These standards are about safety. Don't break them without being really clear on exactly why you're doing it. I don't want to take the fun out of your project, but would rather not read about you in the next Darwin awards either

Lastly, the drive circuitry is actually relatively low impedance, and moves a decent whack of current - 300mA change / up to 750mA discharge. Thicken the trace a little and add a damping resistor right next to the gate itself (between gate and ground) to damp any ringing between the capacitance of the gate and any trace inductance. Ballpark 1k-5k without doing any proper thinking about it.

HTH