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.
Where symbol package (footprint) origin (datum) should be placed?
I decided to be consistent and I place it always at pin 1 of the footprint for both through hole and SMD footprints.
Is it the best location?
I understand that the origin location matters when selecting or moving footprint on a board.
How footprint origin location effects generation of pick and place machine coordinates?
Does origin location matters in this case?
Using Pin 1 for the symbol origin on Thru Components is normally a good thing to do but I would recommend using the centroid or center point for SMD Components. Certainly, being consistent is always the best way to go.
For the most part the origin location doesn't really matter too much in regards to the Pick and Place machine coordinates. The body center information is driven by the calculated center point of the shape defined on Package Geometry > Place_Bound_Top but this can be overriden by defining the component centroid using Package Geometry > Body_Center, normally by adding a text sting like a period "," at the desired center point. This will give you a consistent location vs. a calcuated one for your pick and place centroid point and it can be easily extracted to generate Pick and Place data.
Hope this helps,Mike Catrambone
In reply to mcatramb91:
In reply to Olek:
I am not familiar with Orcad Layout but I believe OrCAD PCB Editor is very similar to Allegro PCB Editor so everything I provided so far is how I have done it inside Allegro PCB Editor.
Its really up to you as far as where the symbol origin is placed. There is some Allegro SKILL Code on Sourcelink that will automatically generate the Body Center for you but I have never used it to give any other further guidance nor do I know if it will run inside of OrCAD PCB Editor.
As far as the Assembly shops placement file, it is best that the placement data does not need any modification or maybe just slight modifications. From past experiences with other companies, clean placement data will make the whole process go much faster and prevents any mistakes that may cost you extra time and money.
You have the ability to output generic placement data from the File menu (File > Export > Placement) and specify whether the data is driven by Symbol Origin, Body Center or Pin 1. Selecting Body Center will use the data provided on Package Geometry > Body_Center first and if it is not present it will calculate the Body Center using the Place_Bound_Top Shape.