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.
A lot of times, especially for prototype circuits, I'll have to include a jumper in a trace. This jumper would have two through hole pads separated by 0.1" and tied together with a copper trace that could be cut during circuit debug / development. Coming from layout, I had a symbol with the two pads and used the "detail" obstacle to create the copper trace between the pads. This worked very well and dod not give me any errors.
That same symbol, now converted to 16.6, gives me DRC's as it sees the trace between the two pads as a short. I sould mention that the schematic symbol is simply two opposing pins with circles and a line between them "symbolizing" the short, there is no real wire connection between the two pins on the schematic. (thus the DRC).
I was wondering how to approach this in 16.6. Could I edit the symbol and put the trace on some alternate layer / class like board geo or pkg goe and then include that class in the gerber generation? I have tried a few things but have had no success, looking for ideas or how thers may have approaced a similar situation.
You could try using the jumper feature. The easiest place I found that describes the feature is the Whats Net in Release 16.3. You can get to that by going to Cadence Help, Whats new for 16.6, then Whats new Older Release. I pasted the doc below.
The use of a wire jumper is sometimes necessary on single-layer PCBs to continue the route over a group of signals; hence the term jumper.
This release offers the following methodology to support jumpers in the Etch Edit environment:
Note: The pop-up menu lists the jumper names stored as drawing properties. Ones that are grayed out either do not exist as a symbol or are not in PSMPATH.
In reply to fxffxf:
fxffxfYou could try using the jumper feature. The easiest place I found that describes the feature is the Whats Net in Release 16.3. You can get to that by going to Cadence Help, Whats new for 16.6, then Whats new Older Release. I pasted the doc below. JumpersThe use of a wire jumper is sometimes necessary on single-layer PCBs to continue the route over a group of signals; hence the term jumper.This release offers the following methodology to support jumpers in the Etch Edit environment:1.Create a package symbol that must consist of two vias.Enable Jumper option in Design Parameter -- Design form (Drawing Type section). of the package symbol drawing.2.Assign the JUMPER_LIST property to the board. This is a drawing level property.The value of the JUMPER_LIST property is a string of valid jumper symbol names.3.When in Add Connect, right-click and choose Add Jumper to add jumper symbol while routing.Note: The pop-up menu lists the jumper names stored as drawing properties. Ones that are grayed out either do not exist as a symbol or are not in PSMPATH.
This only seems to apply to a jumper used when routing a single sided board. When you have to "jump" over a trace, or group of traces as you manually route. You would route up to the group, then select add jumper, and then pick up on the other side of the group.
I'm looking to use a library symbol that has two pins shorted which can be cut if needed during development. For now I will just short the two pins together on the schematic so the netlist has the two pins electrically connected while I work on a scheme similar to what I had done in Layout.
The first picture is the schematic as drawn and goes with the snapshot of the board layout in the first post. The second picture is what I'm doing in the schematic to make it work while I work on a more elegant solution.
In reply to TH Designs:
It can be used to jump over traces since the trace that connects the 2 pins of the jumper is on a virtual layer and you can run traces that fits between the 2 pins of the jumper symbol.
Tom Allegro doesnt handle this very well. It is expecting to see one pin per net. Only way I know to do it is create a 2 pin symbol in capture that looks like a standard jumper and then short those two pins out with a wire in capture. Over on the board side you should be able to route those two pads on your jumper part together. Not ideal but the netlist will match the schematic.
Only other way as you suggested is to use an alternate class layer and put a line between the 2 jumper pins/pads but chances are it might be easy to foregt to turn that layer on in the gerber creation, so no short..
What I have done in the past is to create a special symbol which has overlapping pads to form the short and to suppress the Pin to Pin DRC by added Symbol Drawing property "NODRC_SYM_SAME_PIN"
Here is a summary of the steps:
Hope this helps,Mike Catrambone