Rigid-Flex PCB Layout Rules to Any PCB Design Engineer
The following Rigid-Flex PCB layout Rules are our rich experience for Rigid-Flex PCB Layout Rules, contact us if you have questions. or you can join the Rigid-Flex PCB group.
1、 Outer layer of Rigid-Flex PCB layout Rules
A. Ring of Rigid-Flex PCB layout Rules
Highfive HDI Rigid Flex Prototype PCB Layout Rules
PTH(copper-plated hole) the welding ring of the hole must be 8 mils larger than the single side of the drilling hole, that is, the diameter must be 16 mils larger than the drilling hole. Ring to Board edge or the edge between rigid and flex is over 10 mil.
For the flexible layer, it best to enlarge the smallest hole ring of electroplated through-hole/via hole as much as possible.
In order to cost down for every rigid-flex. It is better to think over how o layout and open windows which can improve the utilization rate of plates. Including Panel Size,
It is best to work together with Mechanical engineers, PCB engineers, PE, ME, QE, etc.
In a word, whether it is a through-hole pad or via hole pad, the setting inner diameter must be greater than 12 mils, and the outer diameter must be greater than 28 mil, which is very important!
Please pay attention to the rigid-flexible boundary, through-hole to plate edge or rigid-flexible boundary, component hole plate edge, or rigid-flexible boundary.
B. Line of Rigid-Flex PCB layout Rules
The line width and line space must be greater than or equal to 4 mils, and the distance between holes shall not be less than 8 mils.
Please design the line perpendicular to the bending axis as much as possible through the line in the flexible area.
The design width changes and vias should be outside the bending area as much as possible.
C. The etching line of Rigid-Flex PCB layout Rules
The etching line width of the outer layer is greater than or equal to 10 mils. It is for etching characters/letters/numbers, but not silk screen printing.
D. The circuit of Rigid-Flex PCB layout Rules
The circuit layer is designed with grid plates (laid in a grid of copper). The rectangle at the grid space is greater than or equal to 10 * 10 mil, that is, when laying copper, the line spacing should not be less than 10 mils, and the grid line width should be greater than or equal to 8 mils.
When laying a large area of copper, it is recommended to set it as a grid, which can prevent the adhesive between PCB substrate and copper foil from generating volatile gas and heat which are not easy to be removed when it is immersed or heated, leading to the expansion and falling off of copper foil; secondly, the heating performance of grid-like flooring, high-frequency conductivity performance is much better than the whole solid flooring.
However, in terms of heat dissipation, the advantages of grid laying copper can not be generalized. In consideration of the deformation of PCB caused by local heating, grid copper laying shall be adopted under the condition of loss of heat dissipation effect and preservation of PCB integrity.
The advantage of this copper laying is that, although the temperature of the board surface has been raised to a certain extent, it is still within the scope of commercial or industrial standards, and the damage to components is limited; however, if the PCB is bent, the direct consequence is virtual Solder joints may directly lead to line failure.
The result of the comparison is to take small damage as the best. The real heat dissipation effect should be solid copper. In practical application, there are few grid-like copper laying in the middle layer, that is, the uneven stress caused by temperature is not as obvious as the surface layer, and the solid copper with better heat dissipation effect is basically used.
E.The distance between NPTH hole and copper of Rigid-Flex PCB layout Rules
The distance between the NPTH hole and copper is greater than or equal to 20 mils.
F. Routing/Milling of Rigid-Flex PCB layout Rules
For the routing/milling cutter outline, the distance between the copper and the outline/boundary of the rigid and flex, which is greater than or equal to 16 mils; therefore, the distance between the line and the edge of the board/boundary of rigid and flex, it shall not be less than 16 mils during layout.
Similarly, when slotting, open window, the distance from copper should be no less than 16 mils.
G. Punching of Rigid-Flex PCB layout Rules
For the die punched boards, the distance between the copper and the outline/boundary of the rigid and flex, it is best over 20 mil or more. If your project would be for mass production later. In order to save costs, it may be required to use mold punching, so it must be foreseen in the design.
H. V-Cut of Rigid-Flex PCB layout Rules
＃The thickness of the V-cut is 1.6mm, and the distance between copper and V-CUT line is greater than or equal to 0.8mm.
＃The thickness of the plate is 1.2mm, and the distance between copper and V-CUT line is greater than or equal to 0.7mm.
＃ The thickness of the plate is 0.8mm-1.0mm, and the distance between copper and V-CUT line is greater than or equal to 0.6mm.
＃ The thickness of the plate is less than 0.8mm, and the distance between copper and V-CUT line is greater than or equal to 0.5mm.
＃The distance between the copper and the V-CUT line is no less than 1.2mm.
Four-layer layout, it is necessary to consider that the flexible area after opening the window can support the shaking of the rigid area during the fab processes. If the window is opened too large, the flexible area will not withstand the shaking of all processes, resulting in abnormalities
2. Inner Layer of Rigid-Flex PCB layout Rules
A. Inner layer of Rigid-Flex PCB layout Rules
The distance between PTH drilling without welding ring in the inner layer and copper foil shall be kept at least 10 mils (four layers) and 11mil (six layers or more).
B. Inner Line of Rigid-Flex PCB layout Rules
When the line width is less than or equal to 6 mils and there are holes in the pad, tears must be added between the line and the pad.
C. Large Copper of Rigid-Flex PCB layout Rules
The isolation area between two large copper surfaces is more than 12 mil.
D. The Cooling PAD of Rigid-Flex PCB layout Rules
For the cooling pad(Quincunx pad), the distance between the drilling hole edge and the inner circle is greater than or equal to 8 mils ( ring), the distance between the inner line and the outer circle is greater than or equal to 8 mils, and the opening width is greater than or equal to 8 mils. Generally, there are four openings, and at least two openings shall be ensured.
3. Drilling Hole of Rigid-Flex PCB layout Rules
A. Slot Hole of Rigid-Flex PCB layout Rules
In principle, PCB factories would change the design “8” shaped holes to slot holes (annular holes). Therefore, it is recommended to make the layout as circular as possible. If there is no such function. You can place more than N circles and stack them as many as possible. In this way, there will be no “dog biting teeth” in the final annular groove, and the PCB manufacturer will not break the drill bit because of your slotted hole.
B.The Minimum Mechanical Hole of Rigid-Flex PCB layout Rules
The minimum mechanical drilling hole diameter is 0.25mm, and the general hole diameter design is greater than or equal to 0.3mm. If it’s smaller than this or just 0.25 mm, the board manufacturer will definitely find you. Please discuss this with the PCB manufacturer if you have any questions.
C. The Minimum Slot Hole of Rigid-Flex PCB layout Rules
The minimum slot hole diameter is 0.25mm, and the general hole diameter design is greater than or equal to 0.3mm.
D. The Laser Hole of Rigid-Flex PCB layout Rules
The laser drilling hole diameter is generally 3mil-8 mil. Generally more than 6 layers, HDI, it will use this technology, of course, the price will certainly increase much more.
For laser drilling, the penetration thickness is less than or equal to 4.5mil, the drilling is a round table hole. So don’t try to use laser drilling technology to PAD. Via holes can be used. So pay attention when placing the pad, and don’t forget the 0.25mm limit.
4. Legend of Rigid-Flex PCB layout Rules
The line width of the text is more than 6 mil, the height of the text is more than 32 mil, and the line width of the text frame is more than 6mil.
5. Hole Copper and Surface Copper of Rigid-Flex PCB layout Rules
- Generally, the surface copper of the finished product is 1 oz, and the hole copper is 0.7mil.
(2) The surface copper of the finished product is 2oz, and the pore copper is 0.7mil-1.4mil.
6. Solder Mask Design Rules
A. It is better than 3 mils larger than the pad. A lot of software is set by default, you can find it yourself.
B.The distance from the anti welding line to copper is more than or equal to 3mil.
C. Solder Mask bridge is over 4 mil, that is, the gap between IC pin anti welding.
D. If the window opening and cover line of BGA position is more than or equal to 2 mils, the Solder Mask bridge shall be designed. If the distance is not enough, the skylight shall be opened.
E. The gold finger part of the gold fingerboard must be anti welding open, including false fingers.
F. In the form of anti welding, the line diameter of characters is over 8 mi, and the word height is over 32 mil.