Cadence® system design and verification solutions, integrated under our System Development Suite, provide the simulation, acceleration, emulation, and management capabilities.
System Development Suite Related Products A-Z
Cadence® digital design and signoff solutions provide a fast path to design closure and better predictability, helping you meet your power, performance, and area (PPA) targets.
Full-Flow Digital Solution Related Products A-Z
Cadence® custom, analog, and RF design solutions can help you save time by automating many routine tasks, from block-level and mixed-signal simulation to routing and library characterization.
Overview Related Products A-Z
Driving efficiency and accuracy in advanced packaging, system planning, and multi-fabric interoperability, Cadence® package implementation products deliver the automation and accuracy.
Cadence® PCB design solutions enable shorter, more predictable design cycles with greater integration of component design and system-level simulation for a constraint-driven flow.
An open IP platform for you to customize your app-driven SoC design.
Comprehensive solutions and methodologies.
Helping you meet your broader business goals.
A global customer support infrastructure with around-the-clock help.
24/7 Support - Cadence Online Support
Locate the latest software updates, service request, technical documentation, solutions and more in your personalized environment.
Cadence offers various software services for download. This page describes our offerings, including the Allegro FREE Physical Viewer.
Get the most out of your investment in Cadence technologies through a wide range of training offerings.
This course combines our Allegro PCB Editor Basic Techniques, followed by Allegro PCB Editor Intermediate Techniques.
Virtuoso Analog Design Environment Verifier 16.7
Learn learn to perform requirements-driven analog verification using the Virtuoso ADE Verifier tool.
Exchange ideas, news, technical information, and best practices.
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.
It's not all about the technlogy. Here we exchange ideas on the Cadence Academic Network and other subjects of general interest.
Cadence is a leading provider of system design tools, software, IP, and services.
I am using Spectre simulator version IC 6.1.5. I know how to set up a initial condition on a node. It can be done in ADE simulation > Convergence Aids > Initial Condition...
Now I am doing a AC simulation and I have a need to set the voltage across a capacitor to zero. The above method will only set the absolute voltage on the node. How to set the delta voltage between two nodes? I searched the Cadence documentation and couldn't get an answer.
Thanks a lot!
Capacitors (at least analogLib cap) provide an "ic" parameter which allows you to do precisely this.
In reply to Andrew Beckett:
OK, I used the "ic" parameter in the AC simulation. When it is done, then I go to Results > Annotate > DC Node Voltages. The voltage shown on the cap is not the voltage I initialized. It seems showing the voltage on the cap in DC condition. Is it right? Also when I go to Results > Annotate > DC Operating Points, it does not show any information (current, voltage) on the cap. The cap is from the "analogLib" library.
Can initial conditions be used in AC simulation? Does it use the initial condition I put in to calculate the AC performance?
I tried it with a simple circuit. Put a voltage source VDC with DC voltage = 3V and AC magnitute =1V. Then connect a diode to it. The anode of the diode connects to the VDC plus terminal. The cathode of the diode connects a 1pF cap. The other end of the cap goes to the GND. The VDC minus terminal goes to GND.
Set the initial condition of the cap to 1V then run a AC simulation. Then change it to 2V, do AC simulation again. I don't see any difference between these two runs. Is it correct? I think it is not because with different operating points, the results should be different.
In reply to apple419:
By default ac analysis doesn't honour initial conditions (nor does dc analysis). You have to add the parameter force=all or force=dev to the ac (or dc) analysis options.
Note that I've not tried your example - but hopefully this will help (I'm a bit pushed for time this week).
I tried what you suggested and it worked!
It is different from PSPICE. Previously with PSPICE the initial condition setting applies to both transient and DC/AC case and I don't need to have to force it. Here with Cadence by default it only applies to transient.
Thanks a lot.
I just try to implement Initial Condition for local PDK capacity for same CDF setting as analogLib cap, even add the parameter force=all but not working for Node Voltage. Is there any thing related to Model File?
In reply to XinjiePI:
I don't think I have enough information to know what your problem is. I think we'd need to see the PDK setup and models - potentially if the device is actually a subckt model, then ic won't work on it. Can you contact customer support so that we can take a look?
Thanks for your quick response.
Actually the model is written as subckt, like:
inline subckt cap (A B SUB)
CAP1 (A B) *******
CAP2 (SUB B) ******
Is that means that ic would not working on it?
Thanks for your comment.
Not unless you create a subckt parameter for the initial condition, and pass it down to the capacitor inside (presumably CAP1 is more important to set than CAP2, but you might need two initial condition parameters).
An "ic" parameter on the instance of the capacitor won't help unless it's consumed within the subckt.