The TI E2E™ design support forums will undergo maintenance from Sept. 28 to Oct. 2. If you need design support during this time, contact your TI representative or open a new support request with our customer support center.

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

LM73605EVM-5V-2MHZ: LM73605 EVM circuit is not able to deliver the rated current of 5A at 5V

Part Number: LM73605EVM-5V-2MHZ

Hello,

Based on this EVM and using the same schematic, I have designed a board. But the max current rating available without voltage fold back is only 3A. Of course,the layout is not exactly same but the circuit is. Any tips on where I could have gone wrong.

Thanks.

  • Hi Ramesh,

    Can you provide the schematic and PCB layout files for review? If you are using the schematic showed in Figure 4 with the exact BOM listed in the Table 3 for 2MHz EVM, then perhaps you are having thermal issues that is limiting your maximum output current. 

    What is your power conditions (VIN,VOUT,IOUT, Tambient)? Can you provide waveforms of VIN,VOUT,IOUT, and SW at no load and full load condition?

    Regards,

    Jimmy 

  • Hi Jimmy,

    Thanks, 

    Vin = 12V, Ta=75F. I am at the lab to take waveforms, but here below is the schematic. If you get any clue with this, let me know.

  • The attachment did not go through, well, I took it from SV601251A.

  • I have chosen BOM for 400KHz version.

  • Hi Ramesh,

    Can you try attaching a compressed folder of your PCB layout design and schematic? 

    It is not visibly showing up on the forum.

    Regards,

    Jimmy 

  • Jimmy,

    I have attached the sch and pcb files.

    PSM_5V_5A E2E.zip

  • Hi Ramesh,

    Just wanted to reconfirm that you are operating at an ambient of 75F and converts out to roughly 24C which is around room temperature. From initial PCB layout inspection, it looks like you have a 2 layer board and only utilizing the single bottom layer as GND for heat dissipation. 

    My thoughts here is perhaps you don't have enough GND copper area for heat dissipation so the output current is limited. The layout example in the datasheet uses a 4 layer board with at least two layers with fully unbroken ground plane. 

    I will continue to review the schematic and PCB design and will add more when I get the chance.

    Please provide the waveform scope-shots when you have them for further review.

    Regards,

    Jimmy 

  • Hi Jimmy,

    Thanks, I was suspecting along these lines as well. Besides being two layer board, the copper thickness is 1oz. Well, when I get to the lab, will attempt to get some plots. In the meantime, if you discover any, let me know.

    Thanks,

    Ramesh

  • Hi Ramesh,

    I checked the schematic and like you mentioned, it is following the 400kHz BOM(specifically Section 4 of guide) so I don't think it is a component selection issue.

    Again this is more likely due GND copper board area for heat dissipation. If you have an infrared thermal camera, can you get thermal measurements of at 12Vin/5Vout/5A?

    Also notice that the EVM uses a 4 layer board that is at least roughly 3000mil x 4000mil (Section 5), while your 2 layer board is measured out to be around 1700mil x 1500mil. Because of this I suspect it is a board heat dissipation issue and you will need to increase your GND board area. 

      

    Regards,

    Jimmy 

  • Would it resolve if I make it 2oz copper on top and bottom and add two inner GND layers to spread the heat out?

  • Hi Ramesh,

    Can you provide the waveform scope-shot first?

    Like I mentioned previously, I'd like to see the VIN,VOUT,IOUT and SW as for 12Vin/5Vout as you increase the output current from 0A to 5A. I am interested to see what the switching waveform looks like as you increase to higher load current. If the voltage folds back at 3A then I'd suspect the SW node to be impacted as well. 

    Right now I suspect the issue is thermal related which is linked to your board area. Giving this waveform will help me get a better understanding of what is happening in your board.

    Regards,

    Jimmy 

  • Hi Jimmy,

    I have uploaded the Vo waveforms with a load of 2E. 004 is with Vi = 21V. 005 is with Vi=12V. For experimentation sake, I increased the Vi to 26V and then got a reasonably flat Vo. I touched on the regulator IC and was not even warm. I cant suspect thermal issue at this point.

    tek00005.zip

  • Hi Ramesh,

    What load current are the two images at? It wasn't clear to me what "load of 2E" means.

    Are you in the lab right now and can you provide the SW waveform at both  Vin = 26V and Vin = 12V at 5A loading? 

    Since the regulator is not hot to the touch then we will need to get more information on what the VIN,VOUT,IOUT, and SW waveform looks like to get a better understanding of what the converter is trying to do.

    Regards,

    Jimmy 

  • A few more comments and questions:

    • Where are you measuring the output voltage at? Are you measuring directly across the output capacitor? 
    • Your feedback trace looks long. It is recommended to reduce that trace by placing the feedback components as close as possible to the IC. Since FB is a sensitive node, long traces act as an antennae that can couple noise into the system and affect regulation. I'd suggest pulling R2,R4,and C15 as close as possible to the FB pin if you plan on redesigning the board. The trace connecting VOUT to RFBT can be long. 

    Regards,

    Jimmy 

  • By 2E, I meant a resistor of 2 ohms is connected at the output for a load current of 2.5A.  Because it is a resistor load,  I did not send the load current waveform as it would follow Vo in shape. Here, am sending the SW at two different voltages (12.5V and 26V). The switching frequency seem to be lesser than 400KHz and there are some narrow spikes showing up, not able to make anything of it.tek00007.zip

  • Hi Ramesh,

    I see you've contacted me offline for this matter. For now let's close this thread and continue with the offline thread.

    Regard,

    Jimmy 

  • Hi Jimmy,

    I reviewed the layout again and realized that the GND plane return path to the device was too narrow. Originally I intended it to be sense/control GND but then it dawned that the freewheeling path has to complete through the device and hence needed a larger plane instead. I shorted the narrow GND plane with larger one across the cutouts and tested it and it was ok.

    Thanks for the time and effort to help me out.

    best rgds,

    ramesh