Under what circumstances is it better to use a hatched (cross-hatched) copper pour instead of a solid fill on a PCB?
For rigid boards, I think that hatched was more useful in the past than these days. If you are concerned about copper balance and having copper regions to etch and plate more like routing areas to avoid warping, this might be a reason. I also think there was a time when users might have been concerned with attempting to force currents over a larger area however most users these days want as much copper as practical for thermal or signal return path reasons. I personally have seldom ever used hatched polygons.
If you are doing flex and need the flex to be as flexible as possible, hatched copper can have real benefits as long as that is more important than signal performance.
Hatched copper will affect impedance calculations so simulation will likely be required as formulas are designed around solid return paths.
3 Likes
I’ll use a hatched copper pour in a flexible or the flex portion of a rigid-flex PCB when I need shielding but want to preserve bendability. The hatching breaks up the copper area, reducing stiffness and the risk of cracking during repeated flex cycles, while still providing enough coverage for EMI control in many applications.
1 Like
In my experience, the only time I find a hatched copper pour truly necessary is in flexible printed circuits. There can be rare cases in rigid boards, such as heavy plating requirements or copper balancing between layers, where hatching might make sense, but these are exceptions. When polygons are adjacent to impedance-controlled traces, hatching generally does more harm than good.
1 Like
Hatched copper pours are commonly used in PCB panelization to achieve proper copper balance across the panel during manufacturing. This helps ensure uniform plating and etching processes around each individual PCB within the panel. Occasionally, you can also use them within individual PCBs to maintain copper balance between layers for stackup symmetry, though in these cases they’re typically not connected to any net.
1 Like
Hatched planes have lower thermal mass compared to solid pours, which can sometimes be beneficial during soldering. With less copper to heat, preheat cycles are shorter, and temperature-sensitive components experience reduced thermal stress. Another side benefit is that solder mask adhesion tends to be better over hatched areas, whereas large solid copper surfaces occasionally risk mask lifting. Historically, hatching was also used for copper balancing between layers, though that’s less of a concern with modern processes.
2 Likes
Back when two-layer boards were the norm, one of the main reasons for using a hatched pour was to help balance copper density between each PCB layer and reduce the risk of warping during fabrication. A hatched pour behaves mechanically more like a set of traces than a continuous copper plane, which made it less prone to stress compared to a solid fill when paired with routing on the opposite side.
In current HDI manufacturing, you rarely see hatched planes used for this purpose, but the same principle of copper balance still applies. Today, fabricators typically add copper thieving (small copper squares or patterns) in unused regions of a PCB layer to equalize plating and etching across the stackup, regardless of PCB copper thickness. This achieves the same effect without the drawbacks of hatching near controlled-impedance or high-speed traces.
2 Likes
An experienced engineer once explained to me that hatched copper pours were sometimes used to mitigate outgassing during wave soldering. When the board was exposed to high soldering temperatures, tiny gas pockets trapped in the fiberglass weave could expand. If these pockets sat under a solid copper area on a PCB layer, the pressure could cause bulging or even delamination of the copper.
Using a cross-hatched pour created small openings in the copper, allowing the gas to escape instead of stressing the plane. Any minor voids left behind could be repaired with solder mask. This practice was more relevant when PCB copper thickness and material quality were less consistent than they are today.
Modern laminates and advanced fabrication processes have largely eliminated this concern, which is why hatched planes are now rarely used in rigid boards except for specific cases like copper balancing or flexibility in flexible PCBs and rigid-flex designs.
2 Likes
When it comes to board warping, is this primarily a fabrication challenge for the board manufacturer, or an issue that also impacts the end-user during assembly and product use? On bigger PCBs or ones with heavy components, I usually just add extra mounting points, is that generally considered enough?
1 Like
It can be a fabrication, assembly, and life of product issue. You really do not want to force a warped board to be straight as the materials will be under internal physical stress for the entire life of the product. This can also lead to component stresses and solder connection stresses which can also fail over time.
3 Likes
Warping can be a major problem in modern SMT assembly. If ceramic MLCC capacitors are soldered onto a PCB that isn’t perfectly flat, and the board is later forced flat when mounted into an enclosure, the mechanical stress can crack the capacitor terminations. Those cracks often turn into latent failures, sometimes short circuits, which are very hard to diagnose.
3 Likes
So does that mean hatched pours aren’t entirely obsolete, but just less common now because modern multilayer stackups and copper-thieving techniques make boards less prone to warping?
1 Like
You’re right, hatched pours aren’t entirely obsolete, but they’re definitely much less common today. The main reason is that multilayer stackups inherently provide better copper balance and structural stability, so warpage is less of a problem. On top of that, printed circuit board manufacturers routinely add copper thieving patterns to unused regions of each PCB layer, which accomplishes the same balancing function without introducing the drawbacks of hatching (like impedance unpredictability or weaker return paths).
So, while you can still see hatched pours in special cases (mainly flexible PCBs, or occasionally in very old-school two-layer designs), they’re no longer part of standard practice for rigid multilayer boards.
2 Likes
Thanks everyone for the detailed explanations. The points on copper balance, warping risks, and why modern multilayer stackups and copper-thieving techniques reduce the need for hatched pours were especially helpful. Now it’s clearer when to use hatching (mainly in flex/rigid-flex) vs. solid fills. Thanks for the insights!
2 Likes
One aspect that hasn’t been mentioned yet is solder mask adhesion. The coverlay or solder mask generally bonds better to bare fiberglass than it does to continuous copper areas. Large, uninterrupted copper pours can sometimes cause the mask to lift or peel over time.
This isn’t as big a problem with modern processes as it once was, but it’s still good practice to avoid very large unbroken copper regions. In fact, it is recommended to introduce small openings in pours larger than about 1″×1 to help the mask lock down and stay in place. A hatched pattern (or even strategically placed breaks) achieves this and reduces the risk of long-term mask adhesion issues.
2 Likes
There are already some great answers here. One niche case I’ve seen for hatched pours is on very thin boards where you need controlled impedance, the hatch changes the plane’s impedance profile enough to let you use wider traces. The trade-off is more crosstalk, strict routing angle limits, and diminishing benefits at higher frequencies. For almost all modern designs, a solid plane is still the better choice.
1 Like