In This Issue

 File Transfers
 By David Moody

 Tooling Package Checklist
 By Robert W. Spaniol

 Lenthor Links

 Presidents Letter
 Words From Mark Lencioni

 Virtual Contacts
 Contact Our Key Employees

 Design Guide
 Download Our Design Guide

 Resources

 Flexible Circuit Materials
 Information on Flex Materials

 Isola Materials
 Rigid Epoxy Material

 Hitachi Chemical Co.
 Rigid Polyimide Material

 IPC Home Page
 Industry Standards

 Newsletter Links

 http://www.lenthor.com
 Lenthor Website

 davidm@lenthor.com
 Contact Us

 Unsubscribe

 Webmaster

In a previous newsletter we looked at what makes up the content of a complete Fabrication Drawing. Many of you responded favorably to that information and asked us to follow it up by providing you the same level of detail for the electronic file transfers. This edition of our newsletter focuses on that topic, the content of a complete file transfer package for the fabrication of your printed circuit design. While the information contained here is primarily directed at what Lenthor Engineering likes to see you can certainly use this as a guideline for any fabricator you may be working with.

The value to you and your fabrication house is great and is the first step you can take to insure a timely delivery of fully compliant product. One note here to direct your attention to the first item listed under “Readme.Doc Requirements”. Though we are sure you will provide a package that is complete in every way having a contact name and number can be very helpful. Many times your design is being reviewed during off-shift engineering personnel. If they have to wait until normal business hours to resolve a question everyone has just lost many hours that could have been used to prepare your job for fabrication. This is very important for jobs being built on an expedited delivery status. In these cases, time really is money.

David Moody
Director Sales and Marketing
Lenthor Engineering LLC

"Tooling Package Checklist."

The following checklist is provided to ensure a complete data package is prepared for file transfer.

Preferred Data Format

• Valor ODB++


• Gerber 274X

Acceptable Format

• Gerber 274D (with standard apertures)

Data Elements
The image is a graphic description of the part used to create the photo tool. The minimum requirements for tooling image data are:

• Inner and Outer layers (all copper layers).
• Soldermask and/or coverlay layers.
• Legend (silkscreen) layers.
• At least one image file supplied for each photo tool with a clear description of the function of each file.
• Image file merging, if required, must be clearly described in a read.me file.
• Aperture list if sending Gerber 274D formatted file.

• If a profile is available in one of the preferred formats, please include it.
• Pads “flashed” with standard aperture shapes rather than “painted” with lines.
• Solid copper areas designated as a “Contour” or “Surface area” versus “painted” with lines. This can be achieved in many CAD systems utilizing correct output parameters.
• If features are painted, an overlap of .5 mil is required.
• Output formats match with Drill output formats (2.4/2.3) to ensure layer/drill registration.
• Use a separate D-code/ aperture for multiple Impedance circuits on the same layer.
• Do not use an output format (2.5, 2.4, 2.3) of lower resolution than the CAD design database; this can cause registration and irregular edges on drawn “painted” features.

• A drill report that includes the following information for each hole size:
• Finished hole size and tolerance (.038” +.003” -.002”) or range .(036”-.041”).
• Quantities for each hole size.
• Hole status (plated, non-plated, via, Press fit, etc.).

• ODB++
• Excellon Format 2
• Gerber 274X

• Gerber 274D (with standard apertures).
• The order of holes in the drill report should match the order in the drill program.
• The drill data shall align with the image data. (Ensure that the output format of the drill file is the same as the image data format (i.e. 2.3, 2.4).
• Plated and unplated holes should be separated into two files.

• Information obtained from the fabrication drawing is used to determine the processes required to manufacture the printed circuit board. The fabrication drawing shall contain the following information as a minimum.
• Bare board part number and revision.
• Board dimensions including the profile, cutouts, chamfers, radii, bevels, scoring, keyways, fiducial locations, slots, and tabs for breakaway rails.
• Dimensions for at least one drilled hole internal to the board.
• Hole chart with symbols matching the drawing with finished hole sizes, tolerances, plating requirements and quantities.
• All requirements for stiffeners (i.e. material, size, location, hole sizes)
• Material requirements.
• Layer stack up.
• Finished board thickness and tolerance.
• Dielectric thickness requirements between layers (if applicable).
• Impedance requirements (if applicable).
• Surface finish requirements (i.e. Soldermask over bare copper).
• Plating requirements for all plated through holes.
• Plating finish requirements with thickness (i.e. solder, nickel/gold).
• Dimensioned array drawing if the parts are to be supplied in multiple up arrays.
• Any specifications to be used while processing the boards.
• Soldermask requirements (i.e. type, color, sides, via plugs).
• Legend (silkscreen) requirements (i.e. type, color, sides).
• Notes defining any special requirements.

• Gerber 274X
• HPGL
• HPGL2

• DXF
• Gerber 274
• Adobe.pdf

Net List Information
It is preferred that customers supply a CAD netlist to be used to check the integrity of the design and to generate the associated electrical test fixture and test program. Preferred format for netlists:

• IPC-D-356

• Contact name and phone number (specify 24 hour contact if different).
• Part number and revision.
• Complete listing of files, drawing and netlist.
• Information on merging files if applicable.
• Special aperture descriptions (thermals, fiducials, etc.).
• File format descriptions.