Can early DFM speed up the production of your PCB?

Author: Craig Haywood, Senior Technical Advisor at Elmatica There are many, many steps in PCB manufacturing and each design needs evaluation during Design Review Checks (DRC’s) including copper distribution, stack up review, inc registration, annular ring compliance and drawing review. This is the tooling time and if the design does not consider all the factors needed to manufacture the PCBs, this can lead to lots of EQ’s possibly meaning lots of delays to board delivery, and inevitable frustrations for customer and manufacturer. So what can we do to prevent this? A good start is DFM (Design for manufacture) as early as possible in the layout stage. Involve the experts to take advice on all topics that could be considered a risk and possibly improve the design. The reduction to EQ's is better for all parties and manufacturers will much rather have a clean data/drawing set that goes straight through DRC’s with minimal EQ’s raised. Check that drawings are up to date with latest information. Elmatica has listed some examples below for your consideration. Stack up – build, materials and laminate thickness Does it need to be a specified build? Standard laminate thicknesses vary by manufacturer. What may be standard for one is non-stock for another. If you do not need specified dielectrics, leave this for the manufacturer to decide. Likewise, does it need to be a specific material type, it is easier to add an IPC rating ie IPC 4101/99/126 to the material option, so the manufacturer is free to choose from available stock. If it is a specified build try to keep laminate thickness the same/similar. Laminates will move differently during the bonding cycle, it is easier for a manufacturer to predict this movement if the laminates are all the same thickness. Is it symmetrical preventing potential bow and twist concerns? Ensure specified prepreg thicknesses are suitable for finished copper thickness i.e. plated layers or copper weights greater than 35um will usually need more prepreg to avoid delamination. Keep the copper distribution balanced and avoid large copper free areas in the build that may lead to low pressure areas during bonding – reduce the risk of panel creasing or delamination. Manufacturers will ask if they can add copper where there is risk of low pressure. Impedance control – are you in control of it? Do you need test results that require coupons on manufacturing panels taking up manufacturing space? Or, if you have a specified build can you accept “impedance by design” and add this note to the drawing? Can you add a note to the drawing confirming the manufacturer is free to adjust tracks/gaps to meet impedance targets?

Craig Haywood

Annular rings The design needs to match the drawing requirement so if you specify IPC 6012 Class 2 or 3 then the drill/pad combination needs to be suitable for the release criteria. Assuming the manufacturer has a registration tolerance of 100um, this then needs to be added to the remaining annular requirement eg 25um Class 2, 50um Class 3. Here’s an example based on drilled size of 300um;

• Class 2 - Drill 300um, pad size should be 550um (125+125um)
• Class 3 – Drill 300um, pad size should be 600um (150+150um)

Ideally pad sizes will increase per bond stage as registration of layers is harder. However in these times where space is limited on boards it is often not possible to utilise such drill/pad combinations. This is pushing manufacturers into smarter bonding systems and use of smaller drill bits. The addition of teardrop fillets to pads is also recommended as this will help meet annular ring requirements. There should also be a safe distance from drilled holes to the nearest copper feature so there is no danger of the drills hitting areas they should not. Typically a distance of 178 to 200um from the edge of drilled hole to copper should be sufficient. Track/gaps Ensure the design measurements are suitable for the copper weight specified. It is unreasonable to think manufacturers can etch high copper weights to define small copper to copper spaces, this will lead to risk of shorts. Number of plating operations also needs to be considered, i.e. through hole, via in pad through vias and microvias can all be present meaning substantial plating requirements. As well as ensuring that track and gap sizes are suitable, and allowing for price and lead time increase for these types of PCBs. Copper up to the board edge will result in exposed copper after routing. If edge plating is not required then copper should be cut back from the board edge to manufacturers capability. Solder Mask Clearances A very common query especially when the distance between surface mount pads are too small to allow a dam of solder mask between them. For green solder mask aim for 50um clearance around pads with at least 75um solder mask dam. Minimum distance between pads ideally is 178um to allow for clearance and dams. Manufacturers have differing capabilities but as a general rule for green solder mask, this distance should suffice. Other colours are available but again, design rules may change/increase, so be careful specifying non-green resist if you only have small pad to pad distances on your design. Silkscreen Silkscreen present on pads is going to lead to the requests to move or clip the legends back. A simple statement on the documentation could erase this EQ. As well as these suggestions for data structure it is important the drawing notes are up to date with latest standards and requirements. Any deviation allowed to drawing notes should be highlighted to prevent additional EQs.

---

Author: © Elmatica's Senior Technical Advisor, Craig Haywood shares some of his advice.