PCB News - General technical standards for circuit board manufacturability design

This standard specifies the general technical requirements for the manufacturability design of single- and double-sided printed circuit boards, including materials, dimensions and tolerances, printed wires and pads, metallized holes, vias, mounting holes, plating, and coating, Characters, marks, etc. As a printed circuit board designer designing single/double sided board (Single/Double sided board) reference:

1 General requirements

As a general requirement for PCB design, this standard regulates PCB design and manufacturing, and realizes effective communication between CAD and CAM.

2 PCB material

2.1 Substrate

The substrate of PCB generally adopts epoxy glass cloth copper clad laminate, namely FR4. (Including single panel)

2.2 Copper foil

a) More than 99.9% electrolytic copper;

b) The thickness of the copper foil on the surface of the double-layer board finished product is ≥35μm (1OZ); when there are special requirements, specify in the drawings or documents.

3 PCB structure, dimensions and tolerances

3.1 Board thickness tolerance

Finished board thickness tolerance

0.4~1.0mm :±0.13mm

1.1~2.0mm :±0.18mm

2.1~3.0mm :±0.2mm

3.2 Overall Dimension Tolerance

The external dimensions of the PCB should conform to the requirements of the design drawings. When the drawing is not specified, the tolerance of the external dimension is ±0.2mm. (Except for V-CUT products)

3.3 Flatness (warpage) tolerance

The flatness of the PCB should meet the requirements of the design drawings. When the drawing is not specified, follow the instructions below

Finished board thickness

0.4~1.0mm

1.0~3.0mm

Warpage

With SMT≤0.7%; Without SMT≤1.3%

With SMT≤0.7%; without SMT≤1.0%

3.4 Structure

a) All relevant design elements that make up the PCB board should be described in the design drawings. The appearance should be uniformly represented by Mechanical 1 layer (priority) or Keep out layer. If it is used in the design file at the same time, generally keep out layer is used for shielding, without opening holes, and using mechanical 1 for forming.

b) In the design drawing, it means to open a long SLOT hole or hollow out, and use MechaNICal 1 layer to draw the corresponding shape.

4 Printed wires and pads

4.1 Layout

a) The minimum drilling tool of our company is 0.3, and the finished hole is about 0.15mm. The minimum line spacing is 6mil. The thinnest line width is 6mil. (But the manufacturing cycle is longer and the cost is higher)

b) In principle, the layout, line width and line spacing of printed wires and pads shall be in accordance with the design drawings. However, our company will deal with the following: appropriately compensate the line width and PAD ring width according to the process requirements. In general, our company will try to increase the PAD as much as possible for the single panel to enhance the reliability of customer welding.

c) In principle, our company recommends that when customers design single and double panels, the inner diameter of the via (VIA) should be set to 0.3mm or more, the outer diameter should be set to 0.7mm or more, the line spacing should be 8mil, and the line width should be 8mil or more. In order to reduce the production cycle to the greatest extent, reduce the manufacturing difficulty.

d) When the design line spacing does not meet the process requirements (too dense may affect performance and manufacturability), our company will make appropriate adjustments according to the pre-manufacturing design specifications.

4.2 Wire width tolerance

The internal control standard for the width tolerance of printed wires is ±15%

4.3 Grid processing

a) The grid spacing is greater than or equal to 10mil (not less than 8mil), and the grid line width is greater than or equal to 10mil (not less than 8mil).

b) In order to avoid blistering on the copper surface during wave soldering and PCB bending due to thermal stress after heating, it is recommended to lay the large copper surface in a grid pattern.

4.4 Treatment of thermal pad

In large-area grounding (electricity), the legs of components are often connected to it. The treatment of the connecting legs takes into account the electrical performance and process requirements to make a cross-patterned pad (heat insulation plate), which can change the cross section during welding. The possibility of excessively dispersing heat and producing virtual solder joints is greatly reduced.

5 Aperture (HOLE)

5.1 Aperture size and tolerance

a) The PCB component holes and mounting holes in the design drawings default to the final finished aperture size. The aperture tolerance is generally ±3mil (0.08mm);

b) The via hole (ie VIA hole) is generally controlled by our company: negative tolerance is not required, and positive tolerance is controlled within + 3mil (0.08mm).

5.2 Definition of metallization (PHT) and non-metallization (NPTH)

a) Our company defaults the following methods as non-metallized holes:

When the customer sets the non-metallized properties of the mounting holes in the advanced properties of Protel99se (remove the plated item in the Advanced menu), our company defaults to non-metallized holes.

When the customer directly uses the keep out layer or mechanical 1-layer arc in the design file to indicate the punching (there is no separate hole), our company defaults to non-metalized holes.

When the customer places NPTH near the hole, our company defaults that the hole is non-metallized.

When the customer clearly requires the corresponding aperture non-metallization (NPTH) in the design notice, it will be processed according to the customer's requirements.

b) All component holes, mounting holes, via holes, etc. other than the above should be metallized.

5.3 Thickness

The average thickness of the copper-plated layer of metallized holes is generally not less than 20μm, and the thinnest part is not less than 18μm.

5.4 Hole wall roughness

PTH hole wall roughness is generally controlled within ≤ 32um

5.5 PIN hole problem

a) The minimum positioning needle of our CNC milling machine is 0.9mm, and the three PIN holes for positioning should be triangular.

b) When the customer has no special requirements, and the aperture in the design documents is less than 0.9mm, our company will add PIN holes at the appropriate positions on the blank wireless road or the large copper surface in the board.

5.6 Design of SLOT hole (slot hole)

a) Our smallest slot cutter is 0.65mm.

b) When opening the SLOT hole for shielding to avoid creepage between high and low voltages, it is recommended that its diameter be above 1.2mm to facilitate processing.

c) It is recommended to use Mechanical 1 layer (Keep out layer) to draw the shape of the slot hole; it can also be represented by a connecting hole, but the connecting hole should be of the same size and the center of the hole should be on the same horizontal line.