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 recently updated to 16.2 capture. I am trying to netlist a design that was done in 16.0
When I netlist, I get the Error [ALG0078] Identical Name property value on two instances in the design.
This previously netlisted OK with 16. I tried to change the name in the property editor, but changes of the name property don't seem to be allowed. I assume these are generated by the tool. The Name property seems to be a truncated version of the instance name.
Is there a way to make the two instances unique? Error log is attached.
Spawning... "C:\OrCAD\OrCAD_16.2\tools\capture\pstswp.exe" -pst -d "Z:\Hw_TITUS\IO_10GE_4pt_module\schematics\rev_08\10g_iom_4pt.dsn" -n "Z:\Hw_TITUS\IO_10GE_4pt_module\schematics\rev_08\allegro" -c "C:\OrCAD\OrCAD_16.2\tools\capture\allegro.cfg" -v 3 -j "PCB Footprint"#1 Error [ALG0078] Identical Name property value "10G_port_no_mux" found on Hierarchical block instances 10G_port_no_mux_p12: H02 - 10G Port, P01_XFP_PHY (5.40, 1.50) and 10G_port_no_mux_p3: H01 - Top Level, P30 - 10G Ports Asymmetric (3.20, 1.20). The value should be unique for correct netlisting.#2 Error [ALG0078] Identical Name property value "10G_port_no_mux" found on Hierarchical block instances 10G_port_no_mux_p12: H02 - 10G Port, P01_XFP_PHY (5.40, 1.50) and 10G_port_no_mux_p3: H01 - Top Level, P30 - 10G Ports Asymmetric (3.20, 1.20). The value should be unique for correct netlisting.#3 Aborting Netlisting... Please correct the above errors and retry.Exiting... "C:\OrCAD\OrCAD_16.2\tools\capture\pstswp.exe" -pst -d "Z:\Hw_TITUS\IO_10GE_4pt_module\schematics\rev_08\10g_iom_4pt.dsn" -n "Z:\Hw_TITUS\IO_10GE_4pt_module\schematics\rev_08\allegro" -c "C:\OrCAD\OrCAD_16.2\tools\capture\allegro.cfg" -v 3 -j "PCB Footprint"
I searched sourcelink for ALG0078 and found the following:
This error appears in case the "Name" property value is identical for one or more instances of a hierarchical block referring to same schematic view. For example, if you have placed two instances of Halfadder block say H1 and H2 in your top level design, the Name property value should be unique for each of the instances say Name = HalfaddedI nst1 for H1 instance and Name = HalfaddedInst2 for H2 instance.
In your case you have a block named 10G_port_no_mux on page 3 of your schematic, and an identically named block on page 12.
Hierarchical block names must be unique. You will have to rename one of the blocks.
I just tried an experiment on a hierarchical schematic and successfully renamed a block with the following proceedure;
1. Left click to select the block.
2. Right click and select edit properties.
3. in column A, select the name field.
4. Delete the existing name, and type a new name.
5. Close the editor
6. Save the page
7. Save the schematic.
This error was fixed in the latest hotfix for OrCAD v16.2. So, install the hotfix (download from downloads.cadence.com) then delete a hierarchical block and copy the existing one and the tool should auto-assign NAME property (it's system assigned). Save, then netlist again. Should work.
In reply to Khurana:
I loaded the hotfix. I didn't want to delete the instance, since that would lose all the reference designators.
I was able to rename the block on H02 and successfully netlist. The trick was to rename at the top level, not the instances.
Thanks for the suggestions.