TPS55165-Q1: Can not get reated power output

Hi Helen,

  Thank you for your help.

   to make things clear, i have attached the detail of PCB and Schematic for all 3 boards i have here.

  Question:

   1. can you help me find out what the reason or biggest effect for this DC/DC when changing the board layout one to another.

   2. from the cost request, we can only do 2Oz copper on top and bottom layer, 1Oz copper for all inner layers, is that good?

  3. i am going to drawing the 4th PCB as a single DC/DC module to put on my product board, can you help me to verify my drawing?

  4. how important to separate the output cap from a 22uF to 10+10+2.2uF?

Thanks and best regards.

Bing Xie

TPS55165 PCB details.docx

Hi Helen,

One thing forgot to ask,

My biggest question is why the 2nd PCB( Product) doesn't work ,which have very similar Layout to the Demo board and Example Layout from TPS55165 data sheet?

Thanks and best regards.

Hi Helen,

Thank you for your quick respond.

1. the request is input between 9~32Vdc, output 12Vdc 800mA.
2. If you looked at the Schematic, you will see, the demo board is using 2 of 22uF caps, and later boards are using 2 of 10uF with 1 of 2.2uF.
I have try the following steps, but doesn't change the result.
i. change the demo board output cap from 0.1uF + 2x22uF to 2.2uF + 2x10uF. Still working well.
ii. change the product board: from 2x10uF +2.2uF to 2x10uF +2.2uF +270uF(HYP). Still not working well.
the output voltage is lower than 12Vdc until input voltage increased higher than 15~16Vdc(Pure buck mode, see it on o'scope screen pics) with 20ohm load( which means about 450mA under 12Vdc output , and less current when output voltage does not meet 12Vdc).
Thanks and best regards,
Bing Xie.

Hi Helen,

for the output cap, OK. the reason to reduced to 2x10uF is based on data sheet suggest. it's ok to put 2x22uF and have a try.
will provide test result to you later.

for he demo board, at about 7~8Vdc input ,with 10Ohm load( 12Vdc output , about 950mA), the input current is higher than 1A, and system still working well.

i do not have tool to measure the inductor current.

the sat current for inductor is 5.9A. just FYI.


Thanks and best regards,
Bing Xie

Hi Helen.

I did a test with the config that all 3 boards have same output cap config, 2x10uF + 1x2.2uF.
The test result is :
The Demo Board: can keep around 950mA output at 12Vdc( 20 Ohm load) , the input voltage range is 8~32Vdc. the output capability is greater than data sheet at 30C room temperature.
The Product Board with 10Ohm load can only provide 12Vdc output when input voltage is higher than around 15~16Vdc. You can check the O'Scope pictures i post in the first question.
The Mini Dc/DC board(3rd), worse than the product board. the output voltage could drop to 0V even without any load for uS level.
Thanks and best regards,
Bing Xie

Hi Helen.

  The following test has done for additional information.

1. Set the Demo board output cap to 2x10uF + 1x0.1uF. does not change the output capability compare to 2x22uF + 1x0.1uF. it's working with 1.15A loads at 12Vdc output with the input range from 8Vdc to 32Vdc.

2. The Mini DCDC Board(3rd) does not work with the same config as the test above. the output drop to 0V for about 20mS often without any load with the config of 2x10uF + 0.1uF output cap.

3. Test the Product Board which better than mini DC/DC but not really working.

*Note: besides the resistor load i put on output side, there are other components liek resistors, OPAMPs and some small DC/DC like TPS 62160 exist, which will use some power.  I have done the test, (take off the inductor of TPS 55165 making this DC/DC stop, wiring a power source to the output side of TPS 55165 directly and record how much current are request when we have so call NO LOAD)

Vout	Iout
V	A
5	0.03
6	0.04
7	0.035
8	0.055
9	0.08
10	0.08
11	0.08
12	0.085

The following test result is what you request, the input current of TPS55165

Load	40	Ohm
Vin	Iin	Vout	Iout
V	A	V	A
6	0.57	9.25	0.221
7	0.51	9.68	0.231
8	0.44	9.85	0.234
9	0.41	10	0.24
10	0.39	10.1	0.242
11	0.34	10	0.239
12	0.33	10.6	0.252
13	0.32	10.6	0.253
14	0.31	10.9	0.26
15	0.31	11.4	0.272
16	0.32	12.1	0.289
17	0.3	12.1	0.289
18	0.28	12.1	0.289
19	0.27	12.1	0.289
20	0.26	12.1	0.289

Load	200	Ohm
Vin	Iin	Vout	Iout
V	A	V	A
6	0.27	9.77	0.045
7	0.24	10	0.047
8	0.21	10.4	0.048
9	0.2	10.8	0.051
10	0.18	11	0.053
11	0.16	10.7	0.05
12	0.17	12.2	0.058
13	0.16	12.2	0.058
14	0.14	11.7	0.056
15	0.14	11.3	0.054
16	0.13	12.1	0.058
17	0.12	12.1	0.057
18	0.12	12.1	0.057
19	0.11	12.1	0.058
20	0.11	12.1	0.058

Load		No load*
Vin	Iin	Vout	Iout
V	A	V	A
6	0.21	12.2	0
7	0.18	12.2	0
8	0.16	12.2	0
9	0.16	12.2	0
10	0.12	10.9	0
11	0.12	11.3	0
12	0.11	12.1	0
13	0.104	12.2	0
14	0.1	12.2	0
15	0.14	12.2	0
16	0.09	12.1	0
17	0.09	12.1	0
18	0.09	12.1	0
19	0.09	12.1	0
20	0.09	12.1	0

Please let me know if you have any questions,

BTW: where are you? are you a Chinese?

Thanks and best regards,

Hi Helen,

A quick question.

 I am drawing the 4th board which seems like the 3rd board(mini DC/DC board) using the suggested 4 Layers board.

Based on the cost request, can i just use 1 Oz for Copper?

and here is my Layout File in PDF, can you help me to check the layout?

Top Layer:Trace and Copper.

2nd Layer:GND

3rd Layer:Vout(12V)

Bottom Layer:GND

to Reduce the total debug time, i'd like to make another PCB very quick, that i can test by next Monday.

Thanks and best regards

Bing Xie

040-000208-a00 rev - evc403-xx8.pdf

GWK1.pdf

Hi Helen,

  I have couple different format of the PCB file attached.

  please let me know if you can open it or not.

if possible, please let me know which format is easy for you to read.

I am using pads 9.5 to do the layout work.

Thanks and best regards,

Bing XiePCB file in different format.zip

Hi Helen.

Forgot to share you that the demo board is a 4 layer 1Oz in each layer board.

the layout see this attach022-000211 Rev X1 Buckboost pushpull flyback powersupply demo bd.pdf

Hi Helen,

  Just get some ideas.

    I think the reason for 4Layers board, one thing important is the impedance of the PCB.

The Demo 4 layers board using typical structure which means it's only a 5mil 2116/7628 between top layer and second layer.

The product board i made is 2.4mm 6 layer even thickness board structure which mean there are 17.523mil (2116+2116H+7628) in betweeen top layer and second layer, which increased the impedance between top layer and second layer.

  and for those high frequency switching power devices, the impedance is very important.

  and this explain that why 2 layer 1.6mm board does not work even without any load.

is the understanding above correct?

Thanks and best regards,

Bing Xie

HI Bing,

1.6mm board should also be OK if the layout is good and the there's no damaged component . I'm wondering if there's some component is damaged? and whether  you use  a high frequency inductor. ferrite inductor is not fit here.

Confirm one thing with you, is my understanding of Vin, Vout right regarding the following picture?

Hi Helen,

1st your understanding of the layout is correct.

2nd.

   I just found something new today, which make me believe the spacing of top layer and second layer is the critical point of making high frequency switching power supply.

  in the product board, there is another DC/DC exist based on TPS62160, to convert 15 V to 3 V, which has tested and passed before.

   Now it's have the issue of

    A. a lot of Vout Ripple without load

  B. under 245mA load, it's still output 4.95V, but the voltage drop to 3.14V @ 302mA.

     And i have the same Schematic and layout in another board which is 2.4mm 6 Layer board, has only 7.337mil spacing between top layer and second layer, the DC/DC ( tps62160) working well at that board.(Tested up to 725mA without voltage drop).

  So i think the spacing between top layer and second layer( gnd) is very important for this switching power supply.

I am modify the layout to 4 layers , put another issued DC/DC together(tps 62160) and targeting is release the board in 12 hours.

Please let me know if you have any questions,

thanks and best regards.

Bing Xie

Hi Helen,

  Thank you for your help.

I have fix this issue.

With the same layout, just increase the layer to 4 ( 4 layers 1Oz PCB), and reduce the spacing between top layer and second layer from about 17mils to about 5 mils make the chip back to work.

I think the independence is the core of the feedback look of those chips( TPS55165 TPS62160)

Again , thank you for your help.

Valve Xie 

Yes.
The second layer is a whole unbroken GND plane.
the core is how far away from the GND plane to the top traces.

Here is the layout. the Vout are came from mian output cap (10uF x 2) and have a 0.1uF to do decoupling , then feedback to chip.

The 3rd plane is Vout and Bottom is empty.

Why doing that? i mean with the GND in the second layer, the system is working . Is there anything i missed?