https://youtu.be/rByRMd7JmTs According to the new definition within IPC-T-50M a microvia is a blind structure with a maximum aspect ratio of 1:1, terminating on a target land with a total depth of no more than 0.25mm measured from the structure’s capture land foil to the target land. The IPC-6012 also defines the structure of a Microvia . The Microvia is a blind structure with a maximum aspect ratio of 1:1 between hole diameter and depth, with a total depth of no more than 0.25 mm , when measured from the surface to the target pad or plane. Typically NCAB considers the dielectric thickness between surface and reference pad to be 60 – 80um. The diameter dimensions of the microvia have a range of 80-100 microns. The typical RATIO is between 0.6: 1 to 1: 1, ideal 0.8: 1 Would you like to learn more about microvias? Read more here

IPC-2226 defines HDI as a printed circuit board with a higher wiring density per unit area than conventional printed circuit boards (PCB). They have finer lines and spaces ≤ 100 µm / 0.10mm, smaller vias (<150 µm) and capture pads <400 µm / 0.40mm, and higher connection pad density (>20 pads/cm2) than employed in conventional PCB technology.

Copper wrap is a continuous deposit of plated copper that is deposited within the barrel of the hole and extends onto the surface of the PCB (or the surface of the innerlayer core if part of a HDI structure) by a minimum of 25 um. For class 2 demands the thickness of the surface deposit of the copper wrap is minimum 5um, but for class 3 demands this will vary dependant upon where this feature is situated within the build. Please consult our technicians for further information on class 3 demands.

PCB Archives

Q: What is meant by a buried via hole?

This is a hole that runs between one or more inner layers. They are normally mechanically drilled. Would you like to learn more about microvias? Read more here

Q: How do you calculate correct length of flex part of a rigid flex structure to allow for minimum bend radius?

Detailed recommendations can be found in IPC-2223, sections 5.2.3.3 for both static and dynamic bends and should be used for final design verification. However, some basic guidelines based upon the thickness of the flex material can be seen below: FLEX TYPE MINIMUM BEND RADIUS Single sided flex 3 - 6 x circuit thickness Double sided flex 7 - 10 x circuit thickness Multilayer flex 10 - 15 x circuit thickness Dynamic application 20 - 40 x circuit thickness

Q: What is the difference between semi-flex and rigid flex?

Semi flex is effectively a ‘standard’ multilayer PCB, built using specific types of FR4 that has been depth to a specific tolerance so that the resulting thinner area provides a flexible / bending section of the traditionally rigid FR4. Semi flex is suitable for static applications (flex to install), or with very limited number of bends.

Q: What is the difference between adhesive and adhesiveless flex systems?

Builds that use adhesive systems rely on adhesive to bond the copper to the flex core. As such this adhesive layer along with full coverlay, penetrates into the rigid construction and directly into the hole. The greater expansion coefficient of the adhesive increases the risk of through hole problems, such as cracks and via hole failures as a result of the expansion, while having this material within the hole itself can lead to hole wall copper formation issues resulting from poor desmear of adhesive. The solution to improving via / through hole reliability was to move towards an adhesiveless copper clad system (copper bonded directly to the polyimide) and limit the overlap of the coverlay into the rigid part of the board. This ensures a much more reliable through hole structure without adhesive penetrating into the hole. This is by far the most common approach to rigid flex.

Q: What is the minimum pad size hole on the outer/inner layer?

This varies from manufacturer to manufacturer, but in general you can say that the majority of manufacturers can produce them as follows: A = 0.15 mm B = 0.20 mm C = 0.30 mm For tighter constructions, please ask one of NCAB's technicians for advice.

Q: When I need thicker tracks than standard, which track widths can I use?

In general, the thicker the copper base, the wider the track should be. One rule of thumb is that with a 18 µm copper base the track should not be narrower than 0.1 mm (4 mil) and with a 105 µm copper base the track should not be narrower than 0.25 mm (10 mil).

Q: Should we remove or keep non-functional pads?

It’s clearly defined in IPC-2222A point 9.1.4 that the fabricator shall not remove these, but many factories ask they allowance to remove these to achieve a better yield in production. If they are not critical for the function, we recommend consider allowing their removal.

Q: What does same net spacing mean?

https://youtu.be/6-CVgGuokKg “Same net spacing” means that the copper to copper distance within the same electrical net is too close to be able to produce according to the Gerber files. Since it is within the same net, the DRC (design rule check) in the customer CAD software doesn´t alarm for this failure. It is important that the customer set the limits correct when starting a new design. Minimum copper to copper distance is normally set up correct, but they miss to set the same value when within the same net. It is not a very big issue, but it causes delay and unnecessary technical questions.

Q: Why is there a demand for such a big distance from hole edge to copper for non-plated holes (NPTH)?

https://youtu.be/Yi71NOcxi3I When you drill holes in the circuit board you want to drill all holes in the same set up to get the best position accuracy for the holes. The non-plated holes needs then to be blocked during the plating process (otherwise they will be plated as well). To be able to block the NPTH we need space between the hole edge and copper. The distance needed is related to the copper thickness. For standard copper thickness (18µm base copper), a good value is 0,3mm and definitely not less than 0,2mm.

HDI

FLEX/RIGID-FLEX

DESIGN RULES

TERMINOLOGY

VIA HOLE

MATERIAL

RoHS