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 doing a PSS+PNOISE simulation of a circuit in Spectre.
I need to multiply the output voltage of certain terminals with Complex Constant ( exp(j*pi/4)=0.707+0.707i).
This I don't want for post-processing ( which can be easily done using Ocean Script).
I want it on the fly of simulation.
Is there any ways of achieving this in VerilogA.
In general, this is impossible in the simulator. This is a constant phase shift of 45 degrees, and that would be non-causal in the time domain.
It could be done in frequency domain analyses only (e.g. ac and hb, including PSS in hb mode), but not by using Verilog-A. Verilog-A cannot be written in the frequency domain - you'd have to translate it into the time domain, and since there is no time domain representation of such behaviour (except maybe over a narrow band), it can't be done that way.
The way I would do this is to create an s-parameter file representing the complex transfer function, and then use nport with this. Be aware though that simulating it in time domain analyses would either fail or give bad answers, as it is not possible in real life. When creating the s-parameter file, you should make sure there is a dc point which doesn't have a complex transfer function (as that's not possible) to ensure the DC behaviour is correct and it can find an operating point.
There is an internal implementation of a phaseShift for SpectreRF use (in frequency domain analyses), but it's not really in a state that I'd want to post it on the forum.
Why can't you do this in the post-processing tool? That works fine - simply multiple your signal by complex(sqrt(2) sqrt(2)) in the calculator.
In reply to Andrew Beckett:
In the earlier post you have mtioned regarding phaseShift for SpectreRF.
Is it now in a state to be used by users like us in PAC & PNOISE analysis.
In reply to RFStuff:
I'm not sure I'd want to post it on the forums - you should contact customer support since we would need to check if R&D are happy to release it to selected customers so that they can give us feedback on how appropriate it is in real life situations.
If you run an ac analysis on a system containing verilogA blocks and use the calculator to implement a multiplier function, is there any way to extract the dc component on the 'multiplier' output? In my example the multiplier inputs have no dc component but the multiplier output will have a dc component. I have simply done a real(VF("/in1")*VF("/in2")) and although I have a result, it does not look correct to me and am wondering about how to fully specify the complex nature of the signals in the calculation.
In reply to J S Mason:
An AC analysis won't give you the DC component as it is a small-signal analysis and there's no DC component at all. It's doing a small-signal linearisation around the DC operating point, and so the complex values you are getting are representing the magnitude and phase of the signals.
You could get the DC component from the dcOp, but to be honest if you're really trying to implement a multiplier, you probably should be using a PSS or HB analysis (maybe with PAC/HBAC afterwards - not 100% sure what your objective is) as this will take into account the frequency translation and non-linear effects that cause the frequency translation.
I am using the ac simulation just to work with ac values so as you say there are no dc components involved. The outputs are two sinusoidal waveforms, one having a phase shift relative to the other, when you multiply these together then there will be a dc component in additional to the ac component.
Using the calculator to do the multiplication should allow this fixed component to measured if the multiplication was actually being done on the two ac inputs as complex variables, eg you were multiplying together Asin(wt) and Bsin(wt-theta) where these represent the multiplier inputs in1 and in2. In the calculator I am doing the multiplication on the signal by using VF("/in1")*VF("/in2") and I am wondering whether this takes into account the complex nature of the two signals fully.
In one of your previous appends you mentioned a complex function and I wondered whether I should be referencing the output signals of the simulation ( in1 and in2 ) in a different way to get a correct multiplication of these complex variables. If this was happening correctly then I think just taking the real component of the output should provide this dc component.
VF() will return the complex waveform versus frequency, and multiplying two complex waveforms together will indeed do a complex multiplication. You can always send the real and imag parts to a table for the input and output waveforms and check the results yourself.
Thanks and I can confirm that it does work, I have tried a real operation on the multiplied VF() waveforms for a simplified testcase and it does return the expected d.c component.