Use of DC operating point parameters in calculations and plots > Forums

Unanswered

Active Topics

Forums

Forums > Custom IC > Custom IC Electrical Design

Subject: Use of DC operating point parameters in calculations and plots

Posting to forums is available to community members only.
Login or Register

Rate this topic:

Author

Messages

axp
Posts: 21
Online: User is Offline

4/17/2007 12:40 AM
Hi all, I run a DC sweep simulation on ADE and I would like to plot some of the DC operating point parameters of my schematic (such as vdsat of the transistors, ...) Moreover, I would like to use these parameters in the calculator in order to make calculations (e.g.: use of vdsat in some calculations). Does anyone have any idea? Thks for considering my request. AXP

adbeckett
Posts: 248
Online: User is Offline

4/17/2007 1:38 AM
This is a very commonly asked question. Create a text file (called, say, saveop.scs) with the following contents: // include file to save op point data save M0:all where M0 is the name of the mosfet. See "spectre -h save" for more details on the save statement. Then, in Setup->Model Libraries, reference this file (I gave it a .scs suffix so it is interpreted in spectre syntax). Run your DC sweep, and then you can access the results via the results browser - or just use an expression such as: getData("M0:vdsat" ?result 'dc) This will then show vdsat versus the swept parameter. The same approach will work if you want to save operating point during a transient - you can always just save the specific op point information by doing: save M0:gm M0:vdsat for example. Best Regards, Andrew.

axp
Posts: 21
Online: User is Offline

4/17/2007 1:43 AM
Thks for your helpful reply!! Regards Axel

axp
Posts: 21
Online: User is Offline

4/25/2007 7:29 AM
A further question... the save statement used in the spectre file, is that a spectreMDL syntax? Where can I find further information on these kind of functions I can use within spectre files? Another question: If I want to create a new symbol whose model is directly a spectre file, what are the steps I have to follow in order to get that model working? I have looked in the analogLib library to get more feeling and examples.However if I look in this library I cannot find any link to a scs file whereas they all link to a spectre analog component. Thks in adv, Regards, Axel

axp
Posts: 21
Online: User is Offline

4/25/2007 8:46 AM
An addition to preceeding message: what do I have to write in order to get the dc operating point from an instance that is inside a subcircuit. I tried to write: save subcktname.M0:all and save subcktname/M0:all as well but it didn't work. Any suggestion?

adbeckett
Posts: 248
Online: User is Offline

4/25/2007 8:59 AM
It's not in spectreMDL syntax - it's just straight spectre syntax. See "spectre -h save" for more details (as I mentioned before). It's also covered in the spectre documentation in cdsdoc/cdnshelp (depending on the version of MMSIM you're using). For hierarchy, you need to use netlist names, and spectre's hierarchy delimiter. So if the transistor is called "M5" and is in an instance called I2, you'd do: save I2.M5:all Note that if M5 is modelled using a (non-inline) subckt model, you would need the name of the instance within the subckt model. The simplest way of finding out (rather than diving through all the model files) is to do a single DC operating point, and then look at the operating point results in the results browser, and see what the instance name there is called. If you want to model something with a subckt model, you can reference that .scs file from the Setup->Model Libraries form in ADE. Then for the component, you can set up the CDF to have the following in the spectre simInfo: componentName: theNameOfTheSubckt termOrder: the order of the terminals in the subckt model, using the names on the symbol instParameters: any parameters you need to pass (need corresponding CDF parameters). You'll also need a stopping view, to tell the netlister to stop expanding the hierarchy at that point. The easiest way to do this is to copy the symbol view to a view called "spectre". Note there are numerous sourcelink.cadence.com solutions on how to do the above, so it's worth looking there if you can. Regards, Andrew.

pdrabos
Posts: 3
Online: User is Offline

7/04/2008 2:30 AM
Hallo, I wanted to do the same thing. I tried this technique what you have recommended, the result is: "Warning from spectre during initial setup. subcktInst:all is not supported. Ignoring invalid item `MN0:all' in save statement." :( it does not work I have check the help and I have tried also: save MN0:oppoint The result: "Warning from spectre during initial setup. subcktInst:all is not supported. Ignoring invalid item `MN0:all' in save statement." :( it does not work What can be the problem? :( br Peter

adbeckett
Posts: 248
Online: User is Offline

7/04/2008 8:41 AM
Did you look at my reply before yours? You must have a subckt model, and so you need to give the hierarchical path (with "." as delimiter) to the actual transistor device. Also, if you use a recent spectre version (e.g. MMSIM621 or MMSIM70) you can save using wildcards (see "spectre -h save" for more details) which makes it easier still. Regards, Andrew.

pdrabos
Posts: 3
Online: User is Offline

7/04/2008 10:05 AM
Posted By adbeckett on 7/04/2008 8:41 AM Did you look at my reply before yours? You must have a subckt model, and so you need to give the hierarchical path (with "." as delimiter) to the actual transistor device. Also, if you use a recent spectre version (e.g. MMSIM621 or MMSIM70) you can save using wildcards (see "spectre -h save" for more details) which makes it easier still. Regards, Andrew. Hi, I do not use any subcircuit, actually I have tried to simulate a very simple circuit: 1 transistor and 2 voltage sources. Does this oppoint depend on the transistor modell? I am using 5.1.41 at the moment... no wildcards :( br Peter

pdrabos
Posts: 3
Online: User is Offline

7/04/2008 10:20 AM
Posted By pdrabos on 7/04/2008 10:05 AM Posted By adbeckett on 7/04/2008 8:41 AM Did you look at my reply before yours? You must have a subckt model, and so you need to give the hierarchical path (with "." as delimiter) to the actual transistor device. Also, if you use a recent spectre version (e.g. MMSIM621 or MMSIM70) you can save using wildcards (see "spectre -h save" for more details) which makes it easier still. Regards, Andrew. Hi, I do not use any subcircuit, actually I have tried to simulate a very simple circuit: 1 transistor and 2 voltage sources. Does this oppoint depend on the transistor modell? I am using 5.1.41 at the moment... no wildcards :( br Peter Hi, So, I have used your method to find how the dc operating values are saved (MN0.m1 in my case) and now it works :). I had to restart ADE, because it did not want to recognize the modification in the scs file. But finally it works. Thanks a lot for your valuable help! br Peter

Posting to forums is available to community members only.
Login or Register

Forums > Custom IC > Custom IC Electrical Design > Use of DC operating point parameters in calculations and plots

ActiveForums 3.6