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.
Is there a way to prevent the netlister from removing parts in the schematic with no pins? We create parts in our schematics that represent the PCB board part number in the BOM and have text in the PCB for symbolization. Is there a configuration to prevent the ALG0060 warning and resultant removal of the part from the Allegro?
Try with the part fixed in Allegro then import netlist. Make sure that Ignore Fixed Property is not checked.
In reply to Khurana:
I am not sure exactly what you are saying. I thought the Fixed Property was in Allegro PCB. I am talking about generating the schematic in Allegro Design and then creating the PCB netlist.
I guess I could instantiate the schematic symbol in Design and load the footprint manually in PCB, but that defeats the purpose.
In reply to mvonahnen:
OK. What are you using for schematic (OrCAD Capture or Allegro Design Entry HDL)? And, what version of the tools are you using? So, you are adding a zero pin part in the schematic? And, you want that part to be included into the netlist for Allegro?
I am using Allegro Design Entry CIS.
The version is SPD 16.01.
I have created a schematic symbol that has no pins and only text to be added to the schematic.
I have created a "Footprint" that contains text on the Top Etch layer and text and shapes on the Top Silkscreen layer.
I would like to have the netlister load the footprint in the PCB when it is instantiated in the schematic, just like other components.
Hmm...the only way I can think of is to use NC pins property to this bogus part - this is required for the part to be "placeable" in Allegro. Otherwise, even if a mechanical part sucessfully made it into the netlist, then Allegro PCB Editor would not allow you to place it since the part is mechanical (i.e. has no pins). The drawback by adding NC pin is that when you run drc then it will say that one is unconnected.
Call Cadence and create an enhancement request.
mvonahnenThis works, but I noticed that this does not work if the pin is a power pin. I could see cases (like mounting holes) where a single power pin device would be desired on a PCB.
Recall that electrical connections such as mounting holes need to appear in the schematic and be attached to a net. We do this all the time for mounting holes -- no issues. Don't use a NC pin for those components.
A non-electrical mounting hole is a different story. You really can't fool Allegro because it'll want the part to be in the netlist but it technically is not in the netlist. Can it be done? See the above poster's comments. It should be a part of the board symbol however....
A serial number label can be brought in as a dummy part but you need to build it like an electrical part to get it go into the netlist. You can turn visibility of pins off to make it appear as if it's not connected. Be sure to X out the pin so the Capture DRC check does not squawk.