Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

a simple resistor noise anlysis

Status
Not open for further replies.
J

John Xu

Member level 3
Member level 3
Joined
Jul 22, 2005
Messages
59
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Activity points
1,938
Hi,
I have a question on below simple resistor noise analysis. PLs. refer below netlist;

***********resistor noise analysis*********
r1 1 0 1K

*vac 2 0 ac 1
*.noise v(1) vac lin 10 1 0.2MEG 1

iac 1 0 ac 1
.noise v(1) iac lin 10 1 0.2MEG 1

.end
***********************

It is just one resistor, I found when I use current AC source, the noise analysis gives correct results. But when I use voltage AC source, the noise is zero.

Can anyone pls. tell me why?

Thanks in advance
 

If your netlist is really the one you've posted, your voltage source (node 2) is not connected to the resistor (node 1). That could be the explaination.
Is it a mistake when copying the netlist?
 

Thanks skal81 point out the typo error. Yes, vac is also connected with "1" node. But the question still exsist. Here I post the netlist again.

***********resistor noise analysis*********
r1 1 0 1K

*vac 1 0 ac 1
*.noise v(1) vac lin 10 1 0.2MEG 1

iac 1 0 ac 1
.noise v(1) iac lin 10 1 0.2MEG 1

.end
***********************

Anyone explain it for me?

Thanks
 

You try to calculate the voltage noise at a node where you assignate a constant voltage.
When you use a voltage source, Spice assign it's value to the node. That's why when it try to calculate the noise after the result is non consistant, leading to zero. With the current source, the current is defined but not the voltage, so calculation is possible.
Try the following:

***********resistor noise analysis*********
r1 1 0 1K
r2 2 1 0

vac 2 0 ac 1
.noise v(1) vac lin 10 1 0.2MEG 1

*iac 1 0 ac 1
*.noise v(1) iac lin 10 1 0.2MEG 1

.end
***********************

By inserting the 0 Ohm resistor you separate the source node and noise calculation node.
I got 1.657567e-012 which is 4kT*1k

Regards.
 

    J

    John Xu

    Points: 2
    Helpful Answer Positive Rating
skal81 said:
You try to calculate the voltage noise at a node where you assignate a constant voltage.
When you use a voltage source, Spice assign it's value to the node. That's why when it try to calculate the noise after the result is non consistant, leading to zero. With the current source, the current is defined but not the voltage, so calculation is possible.
Try the following:

***********resistor noise analysis*********
r1 1 0 1K
r2 2 1 0

vac 2 0 ac 1
.noise v(1) vac lin 10 1 0.2MEG 1

*iac 1 0 ac 1
*.noise v(1) iac lin 10 1 0.2MEG 1

.end
***********************

By inserting the 0 Ohm resistor you separate the source node and noise calculation node.
I got 1.657567e-012 which is 4kT*1k

Regards.
Click to expand...

I tried this simulation.But my simulation results gives the total output noise is 3.3151e-19 V*V/Hz instead of 1.657567e-12, while the current source iac gives the 3.3151e-12 V8V/Hz. It is different. But the output noise should be same, right?

Can anyone pls. explain it?


thanks
 

First I apologize for the input miss yesterday. The result is 1.657567e-17 V^2/Hz (4kT*1k). This is the noise density. If you multiply by the bandwidth of analisys, is 0.2MHz, you'll get the noise power: 1.65e-17*0.2e6 = 3.31e-12 V^2, which is your result for the current source. The unit is V^2, not V^2/Hz.

For the voltage source, it seems that the 0 Ohm resistor is not exactly 0. Some spice version can't handle it properly and put a non-zero value. Here it seems to be 0.0001 Ohm. It leads to the 3.3151e-19 V^2 noise power (1.657575e-024 V^2/Hz noise density).
1.65e-24 = 1.65e-17*0.0001/(1000+0.0001)

I'm sorry but I don't know how to solve this problem. You should check your spice documentation for 0 Ohm resistor.
Which spice do you use?
 

    J

    John Xu

    Points: 2
    Helpful Answer Positive Rating
skal81 said:
First I apologize for the input miss yesterday. The result is 1.657567e-17 V^2/Hz (4kT*1k). This is the noise density. If you multiply by the bandwidth of analisys, is 0.2MHz, you'll get the noise power: 1.65e-17*0.2e6 = 3.31e-12 V^2, which is your result for the current source. The unit is V^2, not V^2/Hz.

For the voltage source, it seems that the 0 Ohm resistor is not exactly 0. Some spice version can't handle it properly and put a non-zero value. Here it seems to be 0.0001 Ohm. It leads to the 3.3151e-19 V^2 noise power (1.657575e-024 V^2/Hz noise density).
1.65e-24 = 1.65e-17*0.0001/(1000+0.0001)

I'm sorry but I don't know how to solve this problem. You should check your spice documentation for 0 Ohm resistor.
Which spice do you use?
Click to expand...

You are right. My simulator is smartspice. I just checked the simulation, it gives the warning"Warning: in r2: resistance reff =0, set to 1e-4/ICG=0.0001
Warning: r2: resistance raceff =0, set to 1e-4/ICG=0.0001", just as you said. It is set 0.0001Ohm in simulation.

I have another question. In the total output noise, I found below informations;
onoise_t.m.xamp1.macs2
onoise_t.m.xamp1.macs2.1overf
onoise_t.m.xamp1.macs2.id
onoise_t.m.xamp1.macs2.rd
onoise_t.m.xamp1.macs2.rs

as my understanding, the "onoise_t.m.xamp1.macs2.id" is the channel noise, while
"onoise_t.m.xamp1.macs2.rd
onoise_t.m.xamp1.macs2.rs" are resistor thermal noise of drain and source's Ohm resistor", then what is "onoise_t.m.xamp1.macs2.1overf"

Thanks
 

I'm not familiar with smartspice, but I would say the onoise_t.m.xamp1.macs2.1overf is the Flicker noise, or 1/f noise. ;)
 

    J

    John Xu

    Points: 2
    Helpful Answer Positive Rating
hi
i dont think so
bye
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top