PCB design doubt

19 posts / 0 new

Hi,
I have a doubt and I'm facing an issue too,

1. when we designing a PCB for flyback LED driver, is there any problem if the MOSFET drain pin and transformer pin distance is about 16mm? I made it like that because I need to accommodate the heat sink!

2. Current sensing Resistor: If the wattage of the current sensing resistor is above the the rated wattage is there any problem? Can I use a single 0.22R 2W resistor instead of 6x1206 chip resistor?

3. I would like to know Ground of the Rcs should be an independent path and how much thickness it has to be needed!?

4. What happens if the snubber circuit is a bit away from the drain pin?

I would be grateful if someone could clear my doubt and help me to improvise the design or to resolve the issues by solutions

Thanks in Advance

Kind Regards
George Thomas

Hi,

So that I can help more effectively, may I ask for the layout pictures and schematic of this particular project you are working on? In the meantime, here's my comments on your inquiries:

  1. 1. For flyback converters, the drain pin of the switch is considered a noisy node (switching at high voltage and frequency). If there is a large distance between the transformer pin and the drain pin, you are introducing a lot of parasitics into your main power loop. It is advised that you keep the main power loop small. This means that the traces should be kept at a minimum and the overall area (input capacitor, transformer, MOSFET switch) kept as compact as possible. As for the heatsink issue, I cannot suggest an alternative placement to this without seeing the actual layout. Perhaps the heatsink can be placed on the source pin instead?
  2. 2. The power dissipated by the current sense resistor (or any resistor) should be less than its rated wattage. For added safety and reliability, this rated wattage should be derated (usually we use 80% derating, meaning for a 2W resistor the maximum power dissipation should be 1.6W). Yes you can use a single higher wattage resistor provided that it is correctly sized and correct value with low tolerance (recommended 1% tolerance).
  3. 3. The current sense resistor is on the main current path therefore its ground connection need not be independent although it should be as near as possible to the output capacitor. Same as the primary loop, the secondary loop should be as small as possible. For the trace thickness, you can use the link provided below to calculate the needed thickness. This can also be used for all other traces in your layout.
  4. 4. For the snubber circuit, it is the same as with the transformer pin and drain pin. You need this loop to be compact as possible. 

PCB Trace Width Calculator: https://www.4pcb.com/trace-width-calculator.html

Dear Sir,
Thank you for the information, This will help me a lot, Sir one more doubt I am having,
1. can take the tracks between the pad of SMD resistor/diode? that too between the gate resistor? 2. My task is to design a single side PCB for the led driver, so for which connection can I use jumpers for interconnection? Can I use jumper to connect feedback pin to feedback resistors?

Dear Sir,
Thank you for the information, This will help me a lot, Sir one more doubt I am having,
1. can take the tracks between the pad of SMD resistor/diode? that too between the gate resistor? 2. My task is to design a single side PCB for the led driver, so for which connection can I use jumpers for interconnection? Can I use jumper to connect feedback pin to feedback resistors?

Hi george,

 

For most cases, it would be fine to route tracks between the pads of SMD components. Still, there are considerations when doing this:

1. The difference in voltage levels in these traces - for safety, you cannot put traces with high voltage differences near each other so if that is the case you cannot route these in between SMD pads.

2. For control section components (ex. feedback, gate drive components, etc.), avoid routing noisy (switching) traces near them to avoid polluting the critical signals they carry.

3. Also, be mindful of the distance between traces. For example, you can route tracks in between a 1206 or 0805 resistor but or a 0603 resistor the pads may be too close for you to route a trace in between.

 

For feedback connection, you can make use of a jumper if there is no better alternative but be sure to place this away from noisy traces or components (ex. output rectifier, secondary winding of transformer). Also, it is recommended that the feedback trace is as short as possible so keep that in mind.

Dear Sir,
Thank you for educating me, I have started to design for new PCB layout, while design I have another doubt.

1. Can I route a 45 degree track for transformer to drain or it should be a straight track?

2. Is there any problem, if I route the primary ground( GND ) and secondary ground ( GND 1 ) track between the transformer? distance between GND and GND1 I kept as 7mm as of now !

3. This question is about the secondary diode ( fast recovery diode ), while I have gone through many manufacturers PSR LED driver reference design and design, I could find designer use different types of diode for same wattage,

Some use MBR1660 or MUR1660, SF56 x 4 in parallel or ES3J x 8 in parallel,
Which one will be the best or good for the LED driver? What is the point of choosing 16A diode for 1A current output ?

Hi george,

 

Here's my comments on your questions:

1. Yes 45 degree bends in traces are okay. The critical thing is actually the length and the width of the trace. Actually it is advisable that when you bend the traces, use 45 degrees angle instead of 90 degrees to avoid sharp edges.

2. Ground traces are quiet nodes (stable voltage level) so putting these traces under the transformer should be okay. 7mm distance should be fine for primary to secondary clearance.

3. In choosing secondary rectifier diodes, here are the main considerations:

  • Peak Inverse Voltage (PIV) - since the voltage on this diode is switching, it is needed to be sized properly for this
  • Reverse Recovery Time (Trr) - it is important that the diode chosen has a fast Trr, preferably use an ultrafast or fast recovery diode.

Usually for a 1A output, a 2A diode should be enough but it depends. Some put a higher rated diode to reduce thermals or to raise efficiency. But I think a 16A diode rating for 1A current output may be too much. Maybe there is some other reason for this that I cannot think of right now. 

Putting multiple diodes in parallel can be done so that you can use lower rated diodes. This works well if you have stringent size constrictions on your design. Still, it is better practice to use a single, correct sized diode than multiple parallel ones due to the fact that parallel diodes do not share current equally and may lead to one diode sinking more current than the other. 

We want to design 98V, 1A (200watt) SMPS to drive LED street light pannel. Please suggest schematic using TOP261YN.

Hi sneha,

Thank you for reaching out to us through this page. However, if may I suggest, can you please create a new thread for this? If you think that this thread is somewhat related to your inquiry then you may include the link in the new thread.

Looking forward on your post.

Thank you and Regards,

PI-Lupin the Third

Dear Sir,
I'm about to finish my design,
I have another doubt now, in many design output / secondary side of the transformer tracks are very solid in shape is square / rectangle with round edges for both negative and positive side to diode and capacitors respectively . what would be the reason for that?

* Whats should be the track width of the output + and - along with capacitor and diode? ( can i follow the same pattern with solid and or the track should be thin? )

* Is it okay, if place the input capacitor after the startup resistor?

Hi george,

Usually solid tracks are used for the tracks of the main current path. This is used instead of just a line to minimize trace resistance. The round edges are preferred because sharp edges may act as an antenna especially for traces with noisy signals.

For the track width, you can follow the solid pattern because this is also a current carrying path. The minimum track width should be given by the PCB trace width calculator which I provided the link for in my first reply. Just input the current, the intended pcb copper thickness, length of trace, and your preferred temperature rise for the specific trace. 

For your last question, I dont understand what you mean by startup resistor. Could you provide a schematic so that I can see which resistor you mean? Thank you. 

Dear Sir,
Its about VCC resistor, which might be of three 200k in series or three 130k in series.
I saw in many PCB layout the after the Cin(Input capacitor) these resistor are placed, but as you mentioned in reply #2 input capacitor, snubber and MOSFET should be kept closer to the transformer!
So is that okay if place the resistor (VCC resistor) layout first and the input capacitor after that.!

Hi george,

Are you pertaining to the input voltage sense resistors? Please see attached image below to see if I understand you correctly.

 

If these are what you are pertaining to, then there is no problem if you place it before the input capacitor as long as it is on the same node. These resistors are used for brown in and to detect input overvoltage scenarios. They only carry very small currents so their traces can be thin. Just make sure to place them away from noisy nodes.

TitleSize
Capture.JPG106.47 KB

Dear Sir,
Literally yes,that's the resistor I mean, as you mention in reply #2 ( point 1 ) if i need to place the input capacitor I have to place it after this resistor layout. I would like to know is that okay or do I need follow the exact order of position as per the schematic?

These queries for academic purpose.

1. Will the current sensing resistor explode , if keep the wattage higher than the desired ?

2. Please find the attachment, What is the need of this circuit ( Fig A ) after the Inductor at the rectifier + ?

TitleSize
Fig_A.jpg27.03 KB

Hi george,

These input voltage sense resistors are not part of the main power loop. They are merely for sensing and input overvoltage protection feature of the IC. It is not strict that you follow the order placement in the schematic. Just keep in mind of each component's purpose when doing the layout.

For example like I said, the components comprising the main power loop should be placed and routed as close as possible. The components carrying critical control signals (ie. feedback, sensing signals) should be kept away from noisy switching traces (ie. MOSFET drain, transformer). Also, you can always refer to the product's/IC's application note on the critical layout considerations. 

 

For your queries:

1. It will not explode, it will be burned due to being unable to handle the power dissipation. But other components might explode if the resistor is damaged.

2.  Where exactly does RECTIFIER+ connect to? Can you give me more snippets of the schematic so that I could better understand the context as to how this particular circuit is being used. Thank you.

Dear Sir,
Thank you for the information.

Answer to 2:
Rectifier + is the bridge output positive ie: 310VDC ( 230Vc input )

I have doubt on 1st explanation, Sir some engineers suggest to keep Through hole current sensing resistor but In our market we can get only 2W resistors, actually 2W resistor is capable to handle the sufficient power dissipation right? Can you help me how to choose the wattage of resistor in LED driver design case and normal DC circuit design case? I'm confused here.!

Kind Regards
George

Hi george,

Sorry for the late reply. I think the attachement shows a peak detect circuit usually for input voltage sensing. 

For the current sense resistors, it depends with what controller you are using. Usually there is a reference voltage the controller uses to regulate the current. For example, for LYTSwitch-6, the reference voltage is at 35.9 mV (based on datasheet with link below). If I am to design a 2 A LED ballast then I would need to calculate my current sense resistors using below equation:

 

Rsense = 0.0359V / 2A = 18 mohms

 

For the power dissipation on this resistor: Pdiss = 0.0359V * 2A = 72 mW

 

So for this particular sense resistor, you can use a 1/4 W resistor.

 

https://led-driver.power.com/design-support/product-documents/data-sheets/lytswitch-6-data-sheet/

Dear Sir,
Thank you so much for the valuable information, In addition I would like to know is there any tutorial or Application note which explains how to design the flyback transformer step by step?

Hi george08,

Thank you for reaching out to us through this page. We are willing to attend to your inquiry, but if you may, please kindly create a new ticket or post for this topic since this is no longer related to your first inquiry.

Looking forward on your post.

Thank you and Regards,

PI-Lupin the Third