Cadence® system design and verification solutions, integrated under our System Development Suite, provide the simulation, acceleration, emulation, and management capabilities.
Verification 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.
The Cadence Academic Network helps build strong relationships between academia and industry, and promotes the proliferation of leading-edge technologies and methodologies at universities renowned for their engineering and design excellence.
Participate in CDNLive
A huge knowledge exchange platform for academia to network with industry. We are looking for academic speakers to talk about their research to the industry attendees at the Academic Track at CDNLive EMEA and Silicon Valley.
Come & Meet Us @ Events
A huge knowledge exchange platform for academia. We are looking for academic speakers to talk about their research to industry attendees.
Americas University Software Program
Join the 250+ qualified Americas member universities who have already incorporated Cadence EDA software into their classrooms and academic research projects.
EMEA University Software Program
In EMEA, Cadence works with EUROPRACTICE to ensure cost-effective availability of our extensive electronic design automation (EDA) tools for non-commercial activities.
Apply Now For Jobs
If you are a recent college graduate or a student looking for internship. Visit our exclusive job search page for interns and recent college graduate jobs.
Cadence is a Great Place to do great work
Learn more about our internship program and visit our careers page to do meaningful work and make a great impact.
Get the most out of your investment in Cadence technologies through a wide range of training offerings.
Overview All Courses Asia Pacific EMEANorth America
Instructor-led training [ILT] are live classes that are offered in our state-of-the-art classrooms at our worldwide training centers, at your site, or as a Virtual classroom.
Online Training is delivered over the web to let you proceed at your own pace, anytime and anywhere.
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.
Get email delivery of the Cadence blog featured here
Some typical questions that I receive from newer SpectreRF users are:
Hopefully the following will help you understand how to do this!
Okay, say you have a transmit mixer. Your IF is 40MHz and your LO is 5.4GHz.
1. First, let's look at the mixing product above the carrier: 5.4G+40M
If you are running PAC or Pnoise, you set the IF sourcetype to dc so that the LO is the only sinusoid in the system (Edit Properties on your IF port in the schematic). Since the input for this example is sinusoidal, we will choose Harmonic Balance.
Set up a pss analysis:
For more information about when to choose Shooting Newton vs. Harmonic Balance, see Solution 11310266.
Set up the Choosing Analysis Form as follows:
Beat frequency= 5.4Goversample=2number of harmonics=5errpreset=moderate or conservative.
For more information on how to set number of harmonics and oversample, please see Solution 11670194.
Next, set up your pnoise analysis.
Here you are specifying an output frequency sweep. Note that by default, the sweeptype is absolute. We want to do a relative sweep, so change the sweeptype to relative and make it relative to the first harmonic. So, we are sweeping output frequency relative to first harmonic from 10K to 100M.
In the example, a log sweep was chosen, with 100 steps. (Note: In practice, 20 steps is probably enough...100 steps may be overkill and will just extend the simulation run time). Set maxsidebands to 5 (same as you had in the pss analysis), choose output voltage (select positive and negative output nets), input source -- port, and select your IF source.
The reference sideband is calculated from:|f(in)| = |f(out) + refsideband*PSSfund|
When you do your sweep, your output frequency will range from 5.4G+10K to 5.4G+100M.
Let's look at one point: 40M refsideband=(fin-fout)/PSSfund= [40M - (5.4G+40M)]/5.4G = -1.
And if you choose "Select from list" in your pnoise Choosing Analyses form, you will see the lower sideband frequencies will be 10K-100M which is the -1 ref sideband. The point is..."Select from List" is your friend. It's easier to use than calculating the reference sideband.
For PAC analysis:
In PAC analysis, we are specifying the input frequency sweep.
Set sweeptype to default (absolute)
Start/stop 10K to 100M, sweeptype log, 100 steps .
f(out) = f(in) + refsideband*PSSfund = 40M + refsideband*5.4G
40M - 5.4G = 5360M (-1)
40M + 5.4G = 5440M (+1)
If we want out output to be 5440M, then we choose the +1 PAC refsideband. In the select from range, that is 5.40001G to 5.5G sweep. Remember: you are specifying an INPUT frequency range in the PAC Choosing Analyses form.
When sweeping output frequency relative to first harmonic from 10K to 100M, you are sweeping from 5.4G +10K to 5.4G+100M.
2. Next, let's look at the mixing product below the carrier: 5.4G-40M.
Remember you are specifying an OUTPUT frequency range in the Pnoise Choosing Analyses form. So, If your output frequency is 5360M (i.e. you are taking the output product on the low side of the LO), then the reference sideband will also be -1. The reference sideband will be: refsideband=[40M -(5.36G+40M)]/5.4G = -1. Again, the "Select from List" is your friend.
Here you would set up the Choosing Analyses form slightly differently (because of limitations in our form).
It would be nice if you could do a log sweep from -10K to -100M with sweeptype=relative, but you cannot at this time. So, you need to do an absolute sweep from 5.3G to 5399.99M.
3. Finally, if you wanted to look at both the upper and lower sideband information...
Sweep from 5.3G to 5.5G as shown in the Choosing Analyses form below. You still choose the -1 reference sideband. Here the frequencies are 100M, 100M. It really should be -100M to 100M.
(We take out the minus sign to make the form less confusing. It makes sense for a receive mixer, but for a transmit mixer, it adds to the confusion factor.)
If you think about it, when you subtract 5.4G (The LO and PSS frequency) from 5.3G (The start frequency) you get -100M.
Note that I have changed this to a linear sweep with 101 points. The reason I didn't use 100 points is because if exactly 5.4M is taken in the pnoise analysis, a warning will be produced that the 1/f noise is being ignored.
4. Setting up the Direct Plot form for Pnoise Separation
You run your simulation and you want to know how to set up the Direct Plot form for Pnoise analysis. When you plot pnoise separation, keep the following in mind.
These two are probably the most useful things to look at:
· Sideband Output plots the noise contribution of selected sidebands to the output.
· Instance Output plots the noise contribution of some instances such as MOS, BJT etc to the output at one selected sideband.
These 4 are a bit more esoteric:
· Instance Source plots the noise sources of some instances at one selected sideband.
· Source Output plots the noise contribution of primary noise source such as re, rb in a BJT to the output at one selected sideband.
· Primary Source plots the primary noise sources such as re, rb in a BJT at one selected sideband.
· Src. Noise Gain plots the noise gains of primary noise sources such as re, rb in a BJT from source to output at one selected sideband.
Note that ViVA/wavescan doesn't tell you which sideband has been plotted. Once you plot the sideband, you need to label it (or remember the order). In your pnoise form, choose select from list and go from 0 Hz to 20G. So, now you may be wondering, "Which sideband should I choose?"
5.4GHz (The center of the output frequency range) minus 5.4GHz = 0 (zero) Hertz. The noise frequencies from -100M to 100M mix up to the output from 5.3G to 5.5G. This is the one you want.
For more tips and tutorials like this, please log into Cadence Online Support (support.cadence.com) .
Have fun simulating!
Very Helpfull for me. Thanks
Hi VJP, Please see the MMSIM13.1 SpectreRF User Guide, Appendix A. There is a more up-to-date (and better) example (documentation and workshop plus database) of simulating a transmit mixer. Best regards, Tawna
Hello Tawna: Could you please report all the component (analogLib) and veriloga (rfLib/mixer) parameter values for the testbench? Perhaps the full netlist would be an easy attachment?
Please see this blog post for more information on the example workshops in the SpectreRF User Guide. www.cadence.com/.../spectrerf-tutorials-and-appnotes-shhhh-we-have-a-new-best-kept-secret.aspx
Please post questions to the general RF community rather than commenting on a specific blog that is from the past. You will get help much more quickly -and- more people will likely see your question. For detailed information and training on the tool, I recommend contacting customer support at http://support.cadence.com. For examples on designing mixers with accompanying databases, please see Appendix A of the SpectreRF User Guide in MMSIM12.1.1 or 13.1. Best regards -- Tawna
I want to design a mixer with specific circuit but I have some problem .
Can you help me?