Design007 Magazine


Issue link:

Contents of this Issue


Page 19 of 89

20 DESIGN007 MAGAZINE I OCTOBER 2018 tions. Is it a starting or finished copper callout? If the part is a multilayer board, is it 2-ounce inners and 2-ounce finished outers? If that's the case, a fabricator will start on 1-ounce copper clad outers and plate to a 1-ounce finish. IPC dictates that there be a minimum of 0.0008" copper in the barrels of the holes for conduc- tivity concerns. Fabricators typically plate up in whole ounce increments to ensure this mini- mum requirement is met, so a part that started on half-ounce copper foil would finish at 1.5 ounces after plate. If a note merely reads 1-ounce finish, the fabricator must call the customer to clarify their intentions because starting on 0.05- ounce foil and plating to 1 ounce does not meet IPC minimum requirements for hole wall thickness. A good copper callout note on a drawing or README file should indicate fin - ished copper for both inner and outer layers as well as a reference to minimum copper in holes, such as: • Copper clad cores and prepregs per IPC-4101/26, 83, 98 • 1-ounce copper weight on internal layers and 0.5-ounce copper plated to 1.5-ounce finish on external layers, unless otherwise specified on stackup This description tells the fabricator a few things at once: • Which materials they are allowed to use (4101/26, 83, 98) • What the inner layer and outer layer starting copper will be, including finished copper For the holes, a good note could read: • All holes to meet IPC-6012B Class 2 annular ring • Plated hole wall thickness to be 0.001" with 0.0008" absolute minimum This callout gives us criteria for acceptabil- ity and a tolerance for hole wall plating. Addi- tional notes about holes could address other items, such as allowed tolerance for true drill position. For example: • All holes shall be located within 0.0008" diameter of the true position Another example might describe whether or not certain hole sizes, such as vias, require conductive or non-conductive filling: • All 0.008" vias to be filled with conductive material and the final surface shall be flat with no dimples or protrusions This is a typical note for via-in-pad appli- cations where the vias are drilled, filled with the conductive material, and planarized (made flat, so that no dimples or protrusions exist on the surface mount). If done right, there will be no evidence that a via even exists in the sur- face mount. If any holes require solder mask plugging or tenting, one might say: • All vias to be filled and covered with solder mask It is important to remember that the absence of such notes on a fairly complicated board can result in a clarification call or email from the fabricator that can delay the fabrication of the parts. Too Much is Just as Bad as Not Enough Is there such a thing as too many notes or details? Yes, an effort to give as much detail as possible can sometimes result in conflicting notes, which will also result in a call or email from your fabricator. For example, one that we frequently need to clarify is where specific dielectrics are shown on a stackup detail on a drawing. In conjunction with this, the notes on the drawing refer to the acceptable types of materials that can be used. The customer will often show a dielectric constant (Dk) value that all impedances are based upon. Many times, the Dk number does not match what the fabri - cator knows to be the real effective Dk of that particular subsection based on the allowed materials and customer-specified dielectric.

Articles in this issue

Archives of this issue

view archives of Design007 Magazine - Design007-Oct2018