How to do this in IC5?

Status
Not open for further replies.
here it is

I call it as 1.scs and put it in my folder in my account i.e as /home/myusername/1.scs

simulator lang=spectre
save NM1ppoint
save NM1:gm


I include this file in the menu path as follows in affirma

setup->simulation files->include path

hope its ok?

I want to plot gm vs Vgs so that I can have some method of choosing the bias point correctly for a so called satisfactory theoretical design as other wise I just feel one plays sort of games with cadence until one gets the required gm!!!
 

Hi,

I have reran the simulation for plotting gm of a transistor and here is a more detailed outline of the procedure. This is done with Analog Artist in IC 5.033.

1. I have created a file - in my case called settings, which content is:

simulator lang=spectre
save M0:gm
save M0:gds

2. Include this file by going to Setup > Simulation files, then click on the Stimulus file field, go to Browse tab and scroll to the file you want to include. Select it, click OK and the absolute path is entered in the Stimulus file field.

3. You can run the simulation now. After it is done, open the results browser: Tools > Results Browser. I have run DC simulation. In this case in the browser left click on psf then on dc-dc, then click on the transistor you want to see gm for and then left-click on gm. This will enter the information for gm in the calculator, if it was opened and you can plot it from there. If you right-click on the gm in the results browser it directly opens the waveform viewer and plots the curve.
The same I can do for gds plot.
That's all.
Hope it is helpful
 
hi sutapanaki,


i am using ic 4.46 of analog artist at school.i guess the "results browser" is well equipped in IC5.03.


i dont find the "psf" ,"dc-dc" stuff in my version

i would greatly appreciate it if u can give me some hint on how to do the gm plot
in the version i have .


thanks a lot for ur time
 

Hi,

I wish I could help you but I did this with 5.033. At work I use 4.46, however the models and simulator are not Spectre, so analog artist changes. I did a quick DC sweep using components of analogLib only. In the results browser I can see /psf -> Run1 and then the analysis I ran. So I guess you should have it too. So much for my help. You should take it from here.
 


Hi sutapanaki
I did it and I feel very good to get the data, now I will go home.
and the only one thing is the manul seem doesn't descripe the element_info
 

you can use result browser
 

Thank all for sharing your knowledge.
A brief summary: some people are using different simulators, so have to handle with different situation. I now could do it in Analog Artist (should select spectre as simulator, not spectreS). SpectreS is quiet stupid to do with some simulations.
One hint from a guy (thanks), should work for standalone spectre simualtion:
put this line in the netlist: "save Melement"
 


I have the same problem, with this save MN1ppoint method.
Do you have any idea, what can be the problem?

Thanks,
 

run sp in spectre, after simulation results->direct plot->main form and you can get gm
 

oermens said:
run sp in spectre, after simulation results->direct plot->main form and you can get gm
Click to expand...

Do you mean make an S-parameter simulation?
 


Problem is solved
 

OK her is may way, you can plot all small signal paramters like gm,gds, cgs, vth and so on. I use ocean for this task. Set a test bench up with one singl Transistor, sweep vgs and set a fix vds. Save the Drain current (select in analogartis save from schematic),this wil give you the right name of the Transistor. Make sure that you on the lowest level, for example if you are on the top of you design the Transistor is calld MN01, but if you go one level down it is called MN01/MN9999 (for example). So here is the trick if you use MN01 as name no gm, but you can still get the Drain current. If you use MN01/MN9999 you get everything you want. You have to figuer out how your Transistor is really called, you should also look at the netlist. When you have save the current, save an ocean skript and change MN01/MN9999.ids into MN01/MN9999.gm and run that skript, I usaly stor the result into a txt fiel and bring it to matlab.
 
Reactions: MFayek

    M

    MFayek

    Points: 2
    Helpful Answer Positive Rating

it's very easy to do that. do DC analysis, then you can find the parameters you interested in the results browser and plot what you want.
 

hi sutapanaki
I have spectre 6.1.1 and
i tried as u suggested but in result browser in psf it only shows variables when i sweep W.
It shows dc-op only when there is no sweep of w.
do i need to check for any other setting ?
Thanks
 


How do you solve it?

Added after 16 minutes:


OK. I also solved it..
Please check your device parameter name.
For me, it should be changed to

simulator lang=spectre
save M0.M1:gm
save M0.M1:gds
save M1.M1:gm
save M1.M1:gds
 
Status
Not open for further replies.

Similar threads

Menu
Log in
Register
Cookies are required to use this site. You must accept them to continue using the site. Learn more…