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.

ft of mosfet nmos pmos 0.18u technology

Status
Not open for further replies.

arunkumar446

Full Member level 3
Joined
Jul 9, 2008
Messages
168
Helped
6
Reputation
12
Reaction score
3
Trophy points
1,298
Activity points
2,198
ft gm cgg

what is the ft of a nmos and pmos in 0.18u technology, and if possible tell me how to measure it using cadence spectre, Thanks in advance.
 

Usman Hai

Full Member level 3
Joined
Apr 8, 2004
Messages
158
Helped
12
Reputation
24
Reaction score
9
Trophy points
1,298
Location
Canada
Activity points
1,230
0.18 technology

ft=gm/2pi*Cgg

Do DC analysis at your desired biasing voltages. Goto simulation, print DC operating point. There you can get gm, and Cgg...you are done!
 

arunkumar446

Full Member level 3
Joined
Jul 9, 2008
Messages
168
Helped
6
Reputation
12
Reaction score
3
Trophy points
1,298
Activity points
2,198
ft in pmos

Thanks for your reply, can you tell me how to plot gm/Id versus vgs in cadence spectre.
 

Usman Hai

Full Member level 3
Joined
Apr 8, 2004
Messages
158
Helped
12
Reputation
24
Reaction score
9
Trophy points
1,298
Location
Canada
Activity points
1,230
nmos-pmos

First connect DC source "Vgs" to an NMOS transistor. Another DC source for Vds and ground to source and connect bulk to source. Now sweep DC Vgs using DC sweep. In order to plot "gmoverid" you need this file.
Please find herewith the stimulus file (It can have any name,. In this case it is "stimulus"). The procedure to use this file with spectre is as follows.

1) Open this "stimulus" file. Here TN1, YN2, TP1, TP2 are the transistor's "instance name". You should replace it with your own instance names. The command "save TN1:all" saves all the DC parameters. The command "save TN2:gm" saves only the gm of the TN2 transistor.

2) On the "Analog Environment" goto "Setup" then "Simulation files" and then on "Stimulus file" add the path of this "stimulus.txt" file.

3) Now do the DC or transient sweep as required (Say you sweep "Vgs" and want a plot of "gmoverid").

4) Now on the "Analog Environment Window" goto "Tools" and then "Results Browser".

5) Click "dc-dc". Here you can see all the saved parameters. Right click "gmoverid" it and plot it.

The file is attached in the button of the post. Just save this text in stimulus file from line "simulator...........".

Please click helped me button if this post is useful to you.

******************
File stimulus
***************
simulator lang=spectre
save TN1:all
save TP1:all
save TN2:gm
save TP2:vth
 

arunkumar446

Full Member level 3
Joined
Jul 9, 2008
Messages
168
Helped
6
Reputation
12
Reaction score
3
Trophy points
1,298
Activity points
2,198
ft for mosfet

hi,
by using the method you suggested for getting ft for an nmos with 400n/180n vgs=1.4 vds=1.8, im getting cgg of 724.522af and gm of 233.635u an ft of 49.125Mhz , instead of getting some thing in GHz's, is there anything im missing, help me with this. Thanks in advance.

Added after 1 hours 47 minutes:

hi, can you tell me one more thing, how to do noise analysis in cadence spectre, i would like to see flicker noise and thermal noise of mosfet, how would be the test bench. Thanks in advance.
 

Usman Hai

Full Member level 3
Joined
Apr 8, 2004
Messages
158
Helped
12
Reputation
24
Reaction score
9
Trophy points
1,298
Location
Canada
Activity points
1,230
cgg spectre

bro! you might missed that aF is 10^-18
So you will get 49GHz, not MHz.
 

arunkumar446

Full Member level 3
Joined
Jul 9, 2008
Messages
168
Helped
6
Reputation
12
Reaction score
3
Trophy points
1,298
Activity points
2,198
ft of mosfet

Thanks Usman Hai, that was a blunder i did. Thanks for the help.

can you tell me about the noise analysis, how to see the flicker noise and thermal noise produced by a mosfet. Thanks in advance.
 

tdf

Member level 2
Joined
Jun 27, 2007
Messages
43
Helped
6
Reputation
12
Reaction score
5
Trophy points
1,288
Location
Vietnam
Activity points
1,520
Re: ft of mosfet

Hi Usman Hai,

Do you know how to measure the Fmax?

It seems that a lot of document that mention the Ft, but the Fmax does not.

Is there any idea with this?

Thanks,
 

turtlewang

Member level 2
Joined
Nov 7, 2010
Messages
46
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,288
Activity points
1,605
Re: 0.18 technology

ft=gm/2pi*Cgg

Do DC analysis at your desired biasing voltages. Goto simulation, print DC operating point. There you can get gm, and Cgg...you are done!

why is Cgg? Why not Cgs in the equation ft=gm/2pi*Cgg?
 

Ramakrishna_444

Member level 2
Joined
Aug 9, 2012
Messages
45
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,288
Activity points
1,609
Re: 0.18 technology

Because Cgg is the capacitance assosiated with the gate terminal.And is equal to Cgs+Cgd+Cgb.
 

beibei

Newbie level 2
Joined
Dec 8, 2012
Messages
2
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,294
Re: 0.18 technology

I use AC and S parameter simulate the ft of NMOS and PMOS in cadence spectre, two kinds of simulation results, then use ft = gm/(2 * pi * Cgg) verify , found simulation of NMOS and calculation results is same, calculation results of PMOS are much smaller than the simulation results, I can get gm, and Cgg using DC analysis. "ft=gm/2pi*Cgg" is suitable for PMOS?
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top