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.
As I'm approaching finishing my first pcb design using 16.5, I have a few questions concerning netlist generation and loading into the board file.
Throughout the board design process, there are occasions where I will need to change the schematic necessitating a new load of the netlist. Coming from the 16.2 and older generation, all I would need to do was "autoECO" the new netlist into the pcb file and keep on trucking.
The process in 16.5 I have to follow is this: (Starting with both Capture and PCB Editor open)
Close PCB Editor
Select the Netlist command in Capture
Pick my board file
Input my output file
Select "Open board in PCB Editor"
This will generate the netlist and open the board in Editor. This seems to be more "manual" then in previous (16.2 and prior) versions. I was not expecting to have to close PCB Editor and manually input the new board file name.
So this begs the question, am I doing this the hard way? Can you have the netlister run while the board file is open AND increment the file name? Older versions would automatically append a -1, 2, etc.... to the board file name.
Not really, if you have a single license for PCB Editor. A license for PCB Editor will be taken if PCB Editor is running, you won't be able to start another PCB Editor session after the netlist is generated unless you have multiple licenses, equally, if you could open two copies of essentially the same board, it might be all too easy to edit the "wrong" one. Also, if the "input" board is open, PCB Editor won't be able to get past the "file lock" to change it.
The name of the input and output boards will be saved in Capture.
The previous "board revision" behaviour was great if that is what you wanted, a real pain if you didn't. You can enable versioning of items in PCB Editor from Setup>User Preferences, File_management, Versioning, ads_boardrevs controls the number of board revisions kept, the default is 1, you can increase this, set the "input" and "output" to be the same in Capture and PCB Editor will look after the file versions when the board re-opens.
In reply to oldmouldy:
Thanks OM. I wasn't looking at having two files open at once as that could become a real issue. I had a designer working for me a few years back that used to do that with 15.7 (I didn't know he was doing it that way) and it got us into a big mess when he renamed components and backannotated the wrong board. But that is a story for another day..........
Being a creature of habit (over 25 years of 16.2 and older use), when I come across something like this, I try to see if I can get it to function the way I'm used to doing it (ie, 16.2 and before). If I can't get it to work that way, then I "conform" and learn the new method. In this case there is no longer an "autoECO" feature like what I was used to in 16.2. So I will close PCB editor, generate the netlist and let Capture open editor back up.
As for the versioning, I'll dig through the info you provided and see what makes sense for me.
In reply to TH Designs:
16.5 introduced file locking so if you editing a board in the PCB editor, the netlist process will report an error since that board is in use.
While file locking can be disabled; it should be considered a good thing because it prevents the loss of edits.
You can change your use model when you know an ECO is available from Capture either by:
I like option 2.
In reply to fxffxf:
Thanks for the tips. The majority of the time, I am the Capture user and Editor user. I usually have Capture on one monitor and the PCB on another. I like being able to volley changes back and forth easily. With 16.5 being the new beast that it is, I just need to learn some new tricks.
PS: Go Phils!
Tom Perhaps this may be an easier way for you.
When your first cut of the schematic is ready to go, in the netlister enter your Imput board file, I usualy use a pre-caned Template with a board outline that has all the layers and colors configured.
Choose your output board name and this will be based on the above template. Run the netlister and package your board. By default I leave the capture option "Do not open Board file" checked as I open Allegro manually.
On your next pass of schematic changes Leave Allegro open but when you go to do the netlist change your input board to your output board name and leave the output board as it is. Check that "Do not open Board file" is enabled and then hit ok to create that updated netlist.
Pop over to allegro and select File "Import Logic" in that window at the bottom choose your import directory to be where your board is packaged then click import logic.
This should update your board for you. From that point on you can go back to capture do a new netlist to update, pop back over to allegro and just hit import logic again to do the updates.
The above works good for me but it is not even close to being as streamlined as the older capture Layout combination. Reminds me of the old PCAD days : )
In reply to ScottCad:
Scott, Thanks for the tip. I have tried it and can see advantages / disadvantages to doing it either way. I need to get through a few more boards to determine what method is more advantagous based on the situation.
Like you said, not nearly as seemless as previous versions. Most of the time I am directly involved in the electrical and packaging design and we end up making changes on the fly fairly often. This is where the seemless-ness of the "autoECO" feature is real useful.
But, at least I'm moving forward. Got my first board done in 16.5. Took about twice as long as it would have using 16.2, but most of that was learning curve. The next job should go quicker as I get more accustomed to the new environment and "lingo".
Hi Tom, nice to hear you got your first board done in 16.5 thats cool. The learning curve on Allegro even for a seasoned pcb designer is a hair-pulling experience. On the up side if you look at the changes Cadence has made since the Allegro 16.2 release and where they are now with 16.6 I think great progress has been made.
Going forward I think they need to get a handle on how they handle libraries for PCB Footprints. As it is right now and if you look at competing tools the lack of a solid Library tool that has good integration with the creation of PCB footprints is a truely glaring omission in my honest opinion. Even the older Layout tool was way better in this regard.
The auto ECO in the older Layout tool was very nice. That took a bunch of grunt work out of the packaging and update process. The import Logic feature in Allegro is kind of similar to that but the only difference is that you have to bit twiddle the files in capture at the front end.