• Skip to main content
  • Skip to search
  • Skip to footer
Cadence Home
  • This search text may be transcribed, used, stored, or accessed by our third-party service providers per our Cookie Policy and Privacy Policy.

  1. Community Forums
  2. Custom IC Design
  3. freq_meter component in ahdlLib

Stats

  • Locked Locked
  • Replies 3
  • Subscribers 124
  • Views 14908
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

freq_meter component in ahdlLib

archive
archive over 18 years ago

Dear all,
 
I'm using freq_meter component from ahdlLib to calculate instantaneous frequency of an oscillator. While doing Spectre simulation, I'm getting the error as
 
==========================================================
Error found by spectre at time = 20.6089 ns during transient analysis `tran'.
    Signal FF(FREQ_OUT) = 2.18688 GHz exceeds the blowup limit for the quantity
       `FF' which is (1 GHz). It is likely that the circuit is unstable. If
       you really want signals this large, set the `blowup' parameter of this
       quantity to a larger value.
==========================================================
 
Please let me know how to resolve this issue.


Originally posted in cdnusers.org by vj
  • Cancel
  • archive
    archive over 18 years ago

    Take a copy of the freq_meter model, and change the section at the top which creates a nature Frequency to the following:

    nature Frequency
    abstol = 1;
    access = FF;
    blowup = 1e12;
    units = "Hz";
    endnature

    The default blowup is 1G, which is a little small if you're measuring frequencies around 1GHz. Note I also increased abstol, since the accuracy requirements shouldn't be so tight if you have GHz signals. Even 1 might be a bit small (normal practice is to set abstol to a millionth of a typical signal level).

    Regards,

    Andrew.


    Originally posted in cdnusers.org by adbeckett
    • Cancel
    • Vote Up 0 Vote Down
    • Cancel
  • archive
    archive over 18 years ago

    Hi,

    I normally find no fault with Andrew's contributions, but I would like to point out that propagating an altered copy of a quasi-standard device from a common library can cause problems if you ever share your schematic with others that don't have access to where you placed the altered copy.  Fortunately, there is another solution which avoids this problem!

    Here's the steps:
    1.  Create a small text file that contains the following lines.
       simulator lang=spectre

       defineLrgFreq quantity                       \
           name="FF"                                     \
           units="Hz"                                      \
           abstol=1e-3                                    \
           description="Frequency in Hz"        \
           huge=100e9
    2.  Save the file with a name like "frequency_nature.scs" in a path that would be accessible to anyone that may end up using your schematic.
    3.  In ADE, do Setup->Simulation Files...  Add the path of the file in Include Path and the name of the file in Defintion Files.

    Now, just leave the freq_meter as is and referenced from the standard ahdlLib.  Netlist and Run will produce a netlist that lets the freq_meter operate at a higher frequency!  Then save a state so that others can recall it and get your modification included already.


    Originally posted in cdnusers.org by SGG_RFIC
    • Cancel
    • Vote Up 0 Vote Down
    • Cancel
  • archive
    archive over 18 years ago

    My practice is to make a local library for the modified elements from bmslib.. and any new ones I create..
    so my first step in making a mod is to copy from bmslib to my local (corporate) lib and make the changes..
    so if they instantiate from the standard lib they get the standard one, otherwise they the the corporate verilog-A/AMS block.
    (which is, of course, under revision control)
    jbd


    Originally posted in cdnusers.org by jbdavid
    • Cancel
    • Vote Up 0 Vote Down
    • Cancel

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.

© 2025 Cadence Design Systems, Inc. All Rights Reserved.

  • Terms of Use
  • Privacy
  • Cookie Policy
  • US Trademarks
  • Do Not Sell or Share My Personal Information