If I understand correctly, I should always create my footprints in metric. In case of a 2.54mm pin spacing (converted parts) I should use a routing grid of 0.01mm to match the pin spacing resolution. Finally, I need to generate my gerber files in metric units with 0.01mm resolution as well.

Thank you for all of your feedback on my questions.
Ed.

The nature of our company is that unfortunately we will be always using mixed technology parts (.100" spacing on connectors, etc..)  with our metric BGA's. However, I will convert all "imperial parts" to metric before saving it to library.

Mixing PCB DesignLayout units will compromise perfection every time. PCB Design perfectionstarts with building CAD library parts and quickly moves to part placement, viafanout and trace routing challenges. Outputting data for machine production canbe extremely complex or very simple based on the PCB Design Layout units thatwere used throughout the PCB design process. One of thesingle most important, but sometimes overlooked or taken for granted, aspectsof the electronics industry is the PCB Design Grid System.

From the 1960’sthrough the 80’s the primary PCB design grid system used Imperial units. AllPCB design features and grid layouts were in 0.001” (1 mil) increments andeverything was symmetrical and evenly balanced. Then in 1988 the worldstandards organizations banded together to agree that the metric unit systemwas superior for solving PCB design development. The first signs of thistransition started appearing in the 1990’s in component manufacturer’s datasheetsand the JEDEC component packaging dimensional datasheets, which were onceentirely based on Imperial “inch” units, where slowly converted to metricunits.

IPC, a worldstandards organization, proposed a base value of 0.05mm for the “PCB DesignGrid System”. And the process of getting all features in the PCB design back “On-Grid” was started. However, this was met by great resistance in the USA. SomeAmerican PCB designers, manufacturing companies, mechanical engineers and EEengineers are still fighting the transition process.

The transition fromone unit system to another introduced chaos in the PCB design industry becausePCB designers were forced into using two different unit systems during thetransition period. The CAD vendor’s way of coping with the transition was tointroduce a “Gridless Shape Based” auto-routing feature that provided the PCBdesigner a solution for working with both metric and imperial unit pin pitchedland patterns. New technical terms were introduced like “Off-Grid” or “Gridless”and “Shape Based” routing solutions. This concept was entirely based on thefact that PCB design rules are the primary factor and the PCB designer’sobjective goal was to adhere to the rules regardless of how irregular the landpattern features were. Some CAD library parts have an inch based pin pitch andsome have a metric pin pitch. The PCB design grid system was chaotic andworking in a gridless environment presented new challenges for PCB designers as well as CAD vendors.

The main impact ofthe gridless system for PCB layout is the fact that trace routing computationsis so granular that it consumes far more memory and CPU processing. Thegridless system has tens of thousands of additional options to commutate andactually slows the auto-routing tools down. It also makes it extremelydifficult to cleanly manually route traces in-between the center of twocomponent leads or vias. The "Enterprise CAD Tools" such as Mentor's Expedition, Zuken's CR-500 or Cadence Allegro are an exception to this rule as they handle gridless computations extremely effienct. All the trace / space rules are defined and that's the only thing that matters for PCB manufacturing. And Expedition has trace / space centering too to add the "Manual Route" look to a PCB layout. However, 90% of all PCB layout companies cannot afford the cost and learning curve of an Enterprise CAD tool. As a matter of fact, most PCB designs are done in CAD tools that cost less than $4,000 USD. These low end CAD tools absolutely need a grid system and most of the trace routing is done manually.

The “Universal PCBDesign Grid System” impacts everything from CAD library creation, partplacement, via fanout to trace routing while at the same time consuming farless computer memory and CPU processing. It also centers traces between pinsand vias increasing manufacturing yields. It also improves the overallaesthetic look of the part placement and trace routing.

The ultimate goal forIPC Standards and designing a perfect PCB is to have all element feature sizesin the PCB design rounded off in 0.05 mm increments and snapped to a 0.05mmgrid system. Note: 0.05mm = 0.0019685” or almost 2 mils

Due to microminiature component packages and smaller tighter PCB layouts, IPC is now considering a shift from the 50um grid system to 10um (high resolution). The new PCB Footprint Expert uses a 10um grid sytem for all PCB library creation to increase the accuracy. 

Tom,

Hello to All,