how to simulate PSRR in bandgap reference?

• Jun 17, 2004

• #1

L

leebluer

Member level 4

Joined

Apr 20, 2004

Messages

76

Helped

5

Reputation

10

Reaction score

3

Trophy points

1,288

Location

China

Activity points

742

how to simulate psrr

how to simulate PSRR in bandgap reference? I think it is different from amplifier. But I don't know the detailed method. Who can give me a clue?

 

• Jun 17, 2004

• #2

H

hylas

Junior Member level 3

Joined

Jun 17, 2004

Messages

25

Helped

5

Reputation

10

Reaction score

0

Trophy points

1,281

Activity points

231

Vdd as AC source,
do .ac analysis (hspice)
probe vdb(vbg)

 

• Jul 8, 2004

• #3

H

hawkin

Newbie level 5

Joined

Jul 5, 2004

Messages

10

Helped

0

Reputation

0

Reaction score

0

Trophy points

1,281

Activity points

84

set VDD ac 1mv
PSRR=dB20(VDD/vout) + DC gain of amp

 

• Jul 9, 2004

• #4

B

billchen

Member level 1

Joined

Jun 18, 2004

Messages

32

Helped

0

Reputation

0

Reaction score

0

Trophy points

1,286

Activity points

321

hawkin said:

set VDD ac 1mv
PSRR=dB20(VDD/vout) + DC gain of amp

Click to expand...

to hawkin
i am confused with u expression，why the DC gain of amp was added to PSRR.i think the dB20(VDD/vout) is ok.

 

• Jul 9, 2004

• #5

H

Hughes

Advanced Member level 3

Joined

Jun 10, 2003

Messages

715

Helped

113

Reputation

226

Reaction score

27

Trophy points

1,298

Activity points

5,984

hawkin said:

set VDD ac 1mv
PSRR=dB20(VDD/vout) + DC gain of amp

Click to expand...

VDD's ac value can be set to 1.0V directly.
PSRR=-dB20(vout)

 

• Jul 9, 2004

• #6

B

billchen

Member level 1

Joined

Jun 18, 2004

Messages

32

Helped

0

Reputation

0

Reaction score

0

Trophy points

1,286

Activity points

321

sorry
i dont understand the difference between them
can u explain it for me
thx very much

 

• Jul 10, 2004

• #7

E

electronrancher

Advanced Member level 1

Joined

Mar 24, 2002

Messages

447

Helped

46

Reputation

92

Reaction score

11

Trophy points

1,298

Activity points

6,935

bill, a simpler way is to just add a 1v AC source on top of your dc source. now your dc sim still works and you can sim AC stuff as well.

the reason you set VAC to 1v is so you can read dB off the plot directly. Now if you have 60dB of PSRR you will see the trace flatten out at -60dB. If you use 1mV then spice gives you this fake, -60mdB number just to make the ratios work out.

it's all relative - you're really not pumping a 1v sine wave into your little circuit, you're just plotting the circuit's response to AC, magnitude = 1.

 

• Jul 11, 2004

• #8

S

staric

Member level 4

Joined

Sep 26, 2003

Messages

79

Helped

4

Reputation

8

Reaction score

3

Trophy points

1,288

Activity points

661

You can refer to the book:CMOS Analog Circuit Design ,Pillips Allen. In the chapter 6, there are many measurement for simulation.

 

• Jul 11, 2004

• #9

B

billchen

Member level 1

Joined

Jun 18, 2004

Messages

32

Helped

0

Reputation

0

Reaction score

0

Trophy points

1,286

Activity points

321

thx to electronrancher and staric!

 

• Jul 12, 2004

• #10

L

leebluer

Member level 4

Joined

Apr 20, 2004

Messages

76

Helped

5

Reputation

10

Reaction score

3

Trophy points

1,288

Location

China

Activity points

742

hello staric, i refer to the book:CMOS Analog Circuit Design by Pillips Allen. but i think the method proposed is for amplifier not for bandgap circuit. the unity-gain struction is suitable for amplifier to measure PSRR, is it true for bandgap circuit?

 

• Jul 12, 2004

• #11

N

nkchenliy

Junior Member level 3

Joined

Feb 11, 2004

Messages

26

Helped

0

Reputation

0

Reaction score

0

Trophy points

1,281

Activity points

147

In fact, in the bandgap circiut, VDD is the input, so you can Vdd as AC source. I always do it as this.

 

• Jul 13, 2004

• #12

H

hanjiemy

Member level 2

Joined

Jun 11, 2004

Messages

53

Helped

0

Reputation

0

Reaction score

0

Trophy points

1,286

Activity points

412

set VDD ac 1mv
PSRR=dB20(VDD/vout) + DC gain of amp

PSRR+ PSRR- (need measure?)

 

• Jul 23, 2004

• #13

M

melodyseu

Junior Member level 3

Joined

Jul 22, 2004

Messages

31

Helped

1

Reputation

2

Reaction score

1

Trophy points

1,288

Activity points

233

hi,Hughes, I think to set ac value to 1v is too large.Although it is convenient to read dB off the plot directly,it may cause other problems especially in low_Vdd cicuit.

 

• Jul 24, 2004

• #14

J

jordan76

Full Member level 3

Joined

Mar 25, 2004

Messages

170

Helped

4

Reputation

8

Reaction score

1

Trophy points

1,298

Activity points

1,852

electronrancher said:

it's all relative - you're really not pumping a 1v sine wave into your little circuit, you're just plotting the circuit's response to AC, magnitude = 1.

Click to expand...

Just as electronrancher explained above.

regards,
jordan76

 

• Jul 28, 2004

• #15

P

piao

Full Member level 4

Joined

Feb 12, 2003

Messages

221

Helped

12

Reputation

24

Reaction score

8

Trophy points

1,298

Activity points

1,517

I think you can refer to Allen's book for the definition of PSRR.

 

• Jul 29, 2004

• #16

H

Hughes

Advanced Member level 3

Joined

Jun 10, 2003

Messages

715

Helped

113

Reputation

226

Reaction score

27

Trophy points

1,298

Activity points

5,984

melodyseu said:

hi,Hughes, I think to set ac value to 1v is too large.Although it is convenient to read dB off the plot directly,it may cause other problems especially in low_Vdd cicuit.

Click to expand...

Hi melodyseu,

It doesn't matter. The AC value and DC value can be set independly. In low_Vdd circuit, the DC value of VDD is low, but its AC value can be any value. The simulator use DC value to calculate the operating point of the circuit. Then all elements are linearized at this operating point. AC simulating is run with the linearized model which will not suffer from saturation problem and the like.

You may do a test. Simulate a simple amplifier with 1mV of AC input value and get the gain: VDB(out)-VDB(in). Then change the AC value of the input to 1000V (This will certainly saturate the amplifier in a REAL amplifier). Do the AC simulation again and get the gain: VDB(out)-VDB(in). You can find the gains obtained from two runs are the same.

 

• Aug 21, 2004

• #17

M

melodyseu

Junior Member level 3

Joined

Jul 22, 2004

Messages

31

Helped

1

Reputation

2

Reaction score

1

Trophy points

1,288

Activity points

233

Hughes,thanks. I think your explain is veyr clear and I got it,
but I still have another question,how to set ac value in the real test?

 

• Aug 22, 2004

• #18

Y

yorande

Advanced Member level 4

Joined

Jan 19, 2004

Messages

104

Helped

1

Reputation

2

Reaction score

0

Trophy points

1,296

Location

China

Activity points

905

Hi, Hughes.
no gain compression in operation amplifiers or bandgaps as it's in the RF circuits?
As I simulated an LNA, it shows the gain compression.

 

• Nov 30, 2004

• #19

always@smart

Full Member level 4

Joined

Feb 8, 2002

Messages

195

Helped

15

Reputation

30

Reaction score

7

Trophy points

1,298

Location

ASIA

Activity points

2,027

dear all,

I've followed what u guys suggested method to measure the bandgap PSRR:

vdd ac=1
.print ac par('vdb(vdd)-vdb(vref)') $plot PSRR

I got the PSRR shown in the graph, is it correct? what is the PSRR value is good for a bandgap?

thanks in advance

 

• Dec 1, 2004

• #20

radiohead

Advanced Member level 1

Joined

May 13, 2004

Messages

447

Helped

66

Reputation

128

Reaction score

31

Trophy points

1,308

Location

Heart of Europe

Activity points

3,562

I have no experience in this, but I don't think that's a great result. 26dB means around times 20 suppression. So a 100mV pulse on VDD (this is possible!) will result in a 5mV pulse on your voltage reference. This does not seem good to me.