Design007 Magazine


Issue link:

Contents of this Issue


Page 55 of 93

56 DESIGN007 MAGAZINE I APRIL 2018 Usable file types for the NC drill file are as follows: 1. Excellon 1 2. Excellon 2 3. An ASCII text drill file a. Note: Please do not mix output formats on the NC drill and route files. Stick with a single convention. For example: 2:4 trailing zero suppression and inch units. Do not mix imperial and metric units on the same file (i.e., inch tool sizes, but with metric increments for position or vice versa). Do not mix formats either (i.e., one file output as 2:4 trailing zero but another in the same output package as 1:5 leading zero). b. If the job has blind vias or epoxy-filled vias that are regional (not all one tool size), please output a separate file denot- ing just hose that need to be filled. The same goes for any blind or buried vias in the design; output a separate NC drill file for each blind or buried scenario that exists. For example: All tools that will go from layers 1-2 of an 8-layer board can be on the same file, but not mixed with other blind vias or through-holes that may be necessary. Drawings in the form of a DXF, PDF or Gerber Drawings should include at a minimum: 1. A board outline with a dimensioned hole or feature plus overall dimensions. This is necessary to be able to place the image within the outline file; many times, the origins of the output files differ. 2. Tool chart showing plating status (plated on non-plated) with tolerances. 3. Material type. 4. Solder mask, ID type, and color, plus any information about minimum or maximum thickness. 5. Surface finish type and thickness plus tolerance. 6. A board stack-up must be included if the board is either impedance or dielectri- cally controlled. Be sure to include copper weights for all layers stated as either start- ing or finished weight. 7. Any required testing notes, such as stan- dard electrical test, IPC netlist compare, etc. 8. Impedance particulars: The width of traces that are controlled, the layers they reside on, the threshold (50 ohms, 100 ohms, etc.), and tolerance. Drawing Confusion Here are some examples of discrepancies or conflicting notes on a drawing that will require clarification: • Example 1: Notes say all inner layers to be half-ounce clad, but stack-up depicting 1 oz. copper internally • Example 2: Notes say all .005" traces on layers 1, 3, 6 and 8 to be 50 ohms. But Gerber image data shows no such size being used • Example 3: NC drill file provided does not match the drawing drill table for either hole count, plating status or hole size As always, a quick cursory look to make sure you have no conflicting notes is advised to min- imize or eliminate delays at the quote stage. IPC Netlists Should you have either an AS9102, IPC class 3 6012 multilayer board, or even just a simple two-layer board and you want to make sure the files emulate the electrical design param- eters, please provide an IPC netlist for net com- parison. As fabricators we are obligated to run an IPC netlist against your provided image data for any class 3 6012 or AS9102 parts, or any parts that specify that a netlist compare must be done on the drawing. What exactly is an IPC netlist? This is an electrical version of your design parameters to be compared with your exported image data. It is not a file to be "generated" by a fabrica- tor based on your image data. If we create a netlist based solely on your Gerber data, at no point would we ever find a mismatch, which

Articles in this issue

Archives of this issue

view archives of Design007 Magazine - Design007-Apr2018