While reading [David L. Jones]'s PCB Design Tutorial, he mentions that hatched polygon pours are a thing of the past.

Solid fills are preferred, hatched fills are basically a thing of the past. (Page 8)

I clearly see the advantage of solid pours over hatched pours: overall better thermal and electrical properties.

But then, why were they so common in older electronics?

Actually, I still see them on some relatively new products¹, so I don't know if it has something to do with industrial etching procedures back in the days, or if it has something to do with EMI.

¹ For example, on a cheap phone charger I took apart the other day.


5 Answers 5


If you are working on say two layers (More common back in the day) you really want to keep the copper density on both sides of the board more or less the same to avoid the thing warping, hatching looks more like tracks then a solid pour does so will suffer less issues if you are doing say route on L2 with a (somewhat broken) ground mesh on L1 .

Even today, when doing HDI boards you will sometimes see extra copper squares added by the board house on unused bits of layers to equalise the overall copper loading.

I would not be shocked if some horribly misunderstood 'skin effect' sort of theory was in play as well.

  • \$\begingroup\$ That means, that in fact hatched pours are not a thing of the past. Only less common as we now work with more layers and our PCBs are therefore less prone to deforming. Right? \$\endgroup\$ Sep 29, 2016 at 16:48
  • \$\begingroup\$ Is board-warping a bigger issue for the board-maker, or the board-user? On big boards, or boards carrying heavy parts, I (as user) simply provide more board mounts-to-chassis. \$\endgroup\$
    – glen_geek
    Sep 29, 2016 at 16:52
  • 3
    \$\begingroup\$ The warping is a huge deal with modern SMT as if you solder down ceramic MLCC caps to a warped board then bolt the thing into a case (forcing it flat) you will very likely crack the cap terminations which has a nasty habit of causing them to fail short circuit at a later date.... The other place you see hatched pours are in flexi circuits where a solid pour tends to make a flexi that doesn't! \$\endgroup\$
    – Dan Mills
    Sep 29, 2016 at 17:33
  • \$\begingroup\$ It is better for galvanic copper plating of a double layer board if the total copper area on both sides is equal. If not, the copper thickness may differ on both sides. \$\endgroup\$
    – Uwe
    Sep 30, 2016 at 12:41

An old-timer EE told me the following while I was learning PCB design...

In years gone by, when manufacturing processes were less advanced than today, the high temperatures involved in wave soldering a PCB would cause gas pockets trapped within the fibreglass weave between the conductor layers to expand. If there was a solid copper plane above the gas pocket then it would bulge out and de-laminate from the PCB.

To rectify this, a cross-hatched plane was used in order to let any gas escape through the tiny holes instead of rupturing the plane. Any damage could quickly be repaired by manually applying solder-mask to fill in the microscopic holes left by the out-gassing.

This is very likely a thing of the past as modern techniques are extremely effective and materials are of a higher quality.


Dan's answer hit the reasons for fills overall, but didn't really address the hatched-versus-solid question.

The main reason is soldermask adhesion- the coverlay does not adhere to copper as well as it adheres to bare fiberglass. As time has gone on, this has become less of an issue, but it is still recommended to not have an area of unbroken copper larger than 1"x1" without some features to allow registration down. There is still an IPC recommendation to have small openings in very large pours to prevent solder mask peel.


Kella Knack on the Altium website has a very detailed explanation on the "The History and Use of Cross-Hatched Planes" which summarizes some of the previous responses.


She says "In the earlier days of the multilayer PCB fabrication process, the final step of inner layer processing involved roughening the copper surfaces so that they would adhere tightly to the resin in the prepreg system during lamination. This step was necessary because the copper surfaces as they emerged from the DES (develop, etch, and strip) process were very smooth. In fact, they were so smooth that it was difficult to create a strong bond between the resin used to laminate the PCB and the copper. As a result, if the copper surfaces weren’t roughened, delamination would occur between the laminate and the solid copper planes of the PCB. This same problem occurred with component mounting pads on outer layers resulting in pads coming loose from the PCB while soldering during rework." ... "To address the foregoing copper adhesion problems on rigid multilayer PCBs, cross-hatching was created. The actual process involved creating small openings in the copper plane so that the resin would bond to the laminate through the copper, rather than attempting to force a bond directly between the resin and copper."

As to why it is still used today, she says "while cross-hatching is rarely used in rigid PCBs these days, it does have practical application for both flex and rigid-flex circuits" ...

  1. Controlled impedance in flex regions: Using a hatch ground is a good method for providing the reference plane required in controlled impedance routing for high speed digital boards." ... "It should be noted that cross-hatching reduces the amount of copper under a transmission line, which decreases the capacitance and raises its impedance." This allows for more trace width/spacing options when dealing with controlled impedance which is useful for rigid PCBs as well.

  2. "Structural support for flex regions: Using a hatch ground provides structural support needed for a dynamic or static flex ribbon without increasing the rigidity of the copper layer. on a two-sided flexible circuit. The layer can still be used for controlled impedance routing creating undesired rigidity, or the ribbon can be permanently deformed."


The reason is the progress of fotoplotters. Decades ago vector fotoplotters with a mechanical apertue wheel were used. They were able to plot pads and traces, but no polygon pours. Therefore the PCB CAD system had to use hatched polygon pours. Now we use raster fotoplotters, they are able to do polygon pours directly without any hatching. Positive and negative plotting is also possible with a raster device, there is no need to copy a film to another one to get a negative.

Even a composite image is possible combining positive and negative parts of the plot. A polygon pour with some isolation gaps for pads within the polygon are very easy this way. In the first step the polygon is rasterized in black (positive), the second step are the isolation gaps as larger pads in white (negative) and the third step are pads itself in black again. If the pads should be round with a diameter of 1.4 mm and the isolation gap is 0.3 mm, the pads in white are 2.0 mm diameter and the pads in black are 1.4 mm. Also isolated traces within a polygon pour are very easy using a raster fotoplotter.

I wish all PCB cad systems would not use hatching any more.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.