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

Help with current mirror simulation

Status
Not open for further replies.
S

sjamil02

Member level 4
Joined
Nov 8, 2009
Messages
72
Helped
9
Reputation
18
Reaction score
5
Trophy points
1,288
Location
United Kingdom
Activity points
1,961
Hi all,

I am running a basic current mirror circuit as shown in the attachment. Reference current is set to ~ 24uA. To set the output current as twice the reference, I need to increase W3/L3 twice bigger than W1/L1. Here's the problem.

In my simulation, W1/L1=3u/3u, M=0, I set W3/L3=6u/3u, M=0. Refer to waveform2 --> Io = 80uA #

Now with same setup, W1/L1=3u/3u, M=0 and I set W3/L3=3u/3u, M=2. Refer to waveform1 --> Io = 50uA # (Close to expected value).

Why there is a discrepancy between those two simulation. My understanding is W3/L3=6u/3u , M=0 same with --> W3/L3=3u/3u , M=2 .......Is it not?

Im confused!

Appreciate any explanation.

cheers
sj
 

Hi,

I am not sure if your M=0 causes the problem. Try replacing it with M=1. Doubling the size makes M=2.

Hope this helps.
 

I am not sure if your M=0 causes the problem. Try replacing it with M=1. Doubling the size makes M=2.
Click to expand...

--> W1/L1=3u/3u, M=1 and W3/L3=6u/3u, M=1 ---> Io= ~80uA

--> W1/L1=3u/3u, M=1 and W3/L3=3u/3u, M=2 ---> Io= ~50uA

Still the same. It looks that the discrepancy came from setting M?

sj[/quote]
 

M=2 is not the same as doubling the width of the transistor (and I am not sure about the idea of using M=0 - unity is more normal).

M=2 assumes two identical transistors are put in parallel - you should be able to confirm that in a simulation. However ift here is a width reduction in the process so 3um drawn ends up as 2.5um, using two in parallel looks like 5um wide wheras drawing 6um wide would result in a 5.5um wide transistor. I hope that makes sense!

What process are you using?

Keith.
 

    S

    sjamil02

    Points: 2
    Helpful Answer Positive Rating
Hi Keith,

Thanks. Yes, you're right. I confimed it in my simulation.

I am using 0.5um technology (level=7) for academic purpose only.
Given in model file, Wint=7.56E-7 and Lint=2.67E-7

Weff=Wdrawn-(2*Wint) and Leff=Ldrawn-(2*Lint)

For Wdrawn/Ldrawn =3um/3um=1 --> Weff/Leff=3um-(2*Wint)/3um-(2*Lint)=0.6


Thanks for your encouraging feedback. I just press helped me button.

cheers
sj
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top