DFM : Tips & Tricks I

- Stipulating a minus tolerance on small (micro) via holes-

This might cause limitations on panel size due to pad/hole ratios. High current densities might plate the hole down. Reworking the vias to unplug the holes is time consuming. Specify if vias can be filled or designate tolerances as a "+" allowance only or specify that vias may be plugged or filled

- Edge Tolerances-

Ground planes (and traces) should end approx 0.010" from the edges of the board to ensure against accidental shorting with metal chassis and cases.

- Nonfunctional pads on inner layers-

Routing traces too close to plated through holes. In designing a board minimum spacing is an important consideration. Often, this spacing does not take into account manufacturing tolerance buildup (ie maximum allowable misregistration combined with maximum etchback). A trace routed between plated through holes on a layer with the nonfunctional pads removed can actually short out during an electrical test resulting in a scrapped unit.

If pads do have to be removed (as is the case in flex or rigid/flex boards) it is advisable to let the manufacturer take care of this.

- Thermal and antipad clearances-

Considering thermals and antipad clearances on the power &/or ground plane layers of multilayer boards - if layer to layer registration, tolerances for hole size, location, film expansion and registration have not been taken into account then manufacturing will experience high reject rates and increased costs.

Antipads should be 0.010 to 0.020" larger than outer layer pads. For thermal pads the moat should be a minimum of 0.012 ( preferable 0.015) and pads should be equal to or larger than outer layer pads.

Clearances for solder masks around non plated holes should be at least .005"

- Restrictive tolerances for multilayer board thicknesses-

Specifying tolerances that are very tight can result in higher costs, increased time and lower yields. It is suggested to call for restrictive tolerances only when they are critical to your design.

- Copper thicknesses-

Often designers request 1 ounce of copper as a finished thickness whether they intend for a copper thickness of that dimension or not. A total of 1 ounce of copper would not ensure adequate plating in the holes. Being specific as to the parameters that you require will ensure that your design will not fail. Common designation for the finished thickness of copper is 1 or 2 ounces per sq ft.

- Providing the Correct Information

One commonly overlooked aspect of board manufacturing is the quality of the information provided to the manufacturer. According to the publication Circuits Assembly, this is the number one cause for extended production cycles and increased costs to the customer. Since cycle time and cost are of considerable importance in today's markets, designers need to have a clear understanding of what is required by their manufacturer.

The first item that is required is, naturally, the artwork. Secondly, the fabricator requires copies of all required specifications and documentation.

Omitting one or more critical elements in the documentation will most certainly create delays in production or affect a products conformance. As a means of addressing this issue, many shops have established mandatory requirement lists and will not send an order to the production floor until all of the requirements are met.

All information must be in a clear understandable format. It must also be complete. CAM editing time can add up quickly and while most operators will make small changes quickly, a design error such as inadequate spacing between components might take hours to correct.

Common problems with a design are incorrectly labled layers, unnecessary pads, hole size changes and minimum space and annular ring violations. In some cases, the design simply does not allow the board to function properly due to connectivity issues or crossed traces.

What would be worse than incurring the added delays or extra costs at this stage, would be the possibility that the errors might not be detected until into production. The results of finding a problem at the production stage will be even more expensive and time consuming.

Some problems in the plating and etching areas of circuit board manufacture result from inadequate spacing between the various artwork elements. Often times, the situation is that the designer is unaware of the clearances that they have built into the design or that they have neglected to advise the manufacturer.

Failing to mention such non conforming design specifications can create very large production problems Spaces dimensions below 0.008" for example can result in incomplete etching and shorts between traces. Etching the boards so that spaces between traces are cleared of metal might result in the traces being over etched and thus not capable of performing as the designer had anticipated.

Performing Design Rules Checks (DRC's) before producing any of the output files are produced should at least alert the designer to potential problem areas. Advising the board fabricator of these concerns allows them take steps to compensate. Referring back to the problem of narrow spaces, a board vendor has the opportunity to over produce the order so to guarantee their yields or to provide further instructions to their staff as how to produce this particular order.

Ideally, the relationship between designer and fabricator should be viewed as a partnership, all parties working together to find ways to meet the demanding requirements of new technologies and market driven manufacturing.