PCB polygon hatched

[electros6]

hi guys,
           In most of the PCB designing tools polygon is provided with solid and hatched. Is there any purpose where solid and hatched should be used.

[tonyarkles]

I don't have a solid reason, but if you're going to end up soldering to the plane, hatched will probably end up being a little easier (less thermal mass).

[elgonzo]

No definite proof here, but there are some arguments that say that hatched pours where used in the past to avoid thermal problems during wave soldering; not only regarding the soldering itself, but also issues regarding "gassing" of the PCB substrate used at that time which could form gas bubbles underneath a solid copper pour.

I remember to have seen a discussion somewhere about how you can control impedance on thin PCBs with crosshatch patterns in certain ways, but that is way beyond my understanding, and i may perhaps remember incorrectly.

[tszaboo]

It is to avoid DFM issues. If your copper distribution is bad, you can fix it by making hatching, so the manufacturer will not under/over - etch your board.
http://www.eurocircuits.hu/index.php/technology-guidelines/pcb-panel-guidelines/96-copper-distribution

[elgonzo]

It is to avoid DFM issues. If your copper distribution is bad, you can fix it by making hatching, so the manufacturer will not under/over - etch your board.
http://www.eurocircuits.hu/index.php/technology-guidelines/pcb-panel-guidelines/96-copper-distribution

The link you have given speaks only about copper fills in general, not specifically about solid vs. hatched fills. There is sole picture picture showing a hatched fill, which doesn't say much, i am afraid

[Dielectric]

Hatched fill reduces parasitic capacitance with traces on another layer.  There's less "coupling" area between your hatch and the active traces.

[mazurov]

Solid pour plus turned off thermals is preferable in DC-DC converters (see, for example, Linear Tech. App.note 136, p.7). Manual soldering will be difficult though.

[tszaboo]

It is to avoid DFM issues. If your copper distribution is bad, you can fix it by making hatching, so the manufacturer will not under/over - etch your board.
http://www.eurocircuits.hu/index.php/technology-guidelines/pcb-panel-guidelines/96-copper-distribution

The link you have given speaks only about copper fills in general, not specifically about solid vs. hatched fills. There is sole picture picture showing a hatched fill, which doesn't say much, i am afraid

The link + Copper distribution. If you fill it 100%, that is bad, if you fill it 0% that is also bad. If you fill it with a ratio, which matches the rest of the PCB than the etching will be better.

[elgonzo]

The link + Copper distribution. If you fill it 100%, that is bad, if you fill it 0% that is also bad. If you fill it with a ratio, which matches the rest of the PCB than the etching will be better.

Now, i have to admit i do not know the details about the etching process (in terms of chemical reaction(s)) and how local variations in available reactants (= copper to dissolve) can have an impact on the overall process. However, i find it odd that i never see crosshatch pours in newer equipment, even if it are sensitive instruments with not-so-even copper distributions on the PCB (just look at Dave's or others teardown videos). If crosshatch patterns are important/recommended for good results during etching as suggested, why are they not being used (not even for thoroughly engineered lab and measurement devices where the small additional design effort could certainly be afforded)? Or is it relevant only for certain border-line cases?

(or perhaps it is just me, never encountering those crosshatches except in older equipment, thanks to the naturally occurring randomness in life... )

[T3sl4co1l]

I often did hatched for toner transfer process.  I suspect it's something to do with the toner density around edges versus inside a fill.  10-30 mil traces, fine, but over 100 mil or so it starts to get spotty, and floods were often crusty (even after filling in with sharpie).

I've only seen hatched PCBs a few times (and the inverse -- thieving on otherwise empty areas -- even fewer), so I don't think it's a big deal either way.

Tim

[TerraHertz]

Another reason for hatching is that large area PCBs with lots of solid copper on one side tend to warp during wave soldering and cooling. Not sure how much of a problem this is with vapor phase soldering, since by then I was always hatching copper areas.

Also with wave soldering, where there are pads and openings in the mask, if large copper areas are pre-tinned before the mask was printed on, solder tends to flow under the mask. Results in both a waste of solder, and unsightly bumps under the mask. Hatching large copper areas stops that by anchoring the mask layer to the fiberglass.
This effect obviously isn't a factor with stenciled application of solder paste and vapor phase soldering.

On the other hand, if you want controlled impedance traces, and best possible ground planing around HF/High current circuits, then it's a tradeoff and sometimes solid copper areas are best.
And presumably high volume PCB manufacturers prefer to minimize copper etch, to get the best life from their etching chemicals.

[tszaboo]

I guess, it is not really an issue for high quality PCB manufacturing. I've seen it being used in some washing machine controller board, or switching power supply . Usually big, cheap, through hole components, often one sided PCB.
Ti recommends the method for their capacitive touch controls also.

[Richard Head]

Another reason for hatching is that large area PCBs with lots of solid copper on one side tend to warp during wave soldering and cooling. Not sure how much of a problem this is with vapor phase soldering, since by then I was always hatching copper areas.
I can second that. I did a large board recently that had a full un-hatched groundplane on one side and no groundplane on the other side. When manufactured it warped like banana. Once I added a polygon pour on the top (and grounded it) it was as flat as a board.

[pilav]

electros6, there is actually not much difference in hatched and solid PCB polygons, it’s just a matter of preference in some cases and in some cases, and there are some manufacturing considerations. By experience, cases have been developed for both types of polygons, they are accurate in suggesting that there might be some parasitic capacitance in some cases but mostly it isn’t enough to be a problem.

[DanielS]

If crosshatch patterns are important/recommended for good results during etching as suggested, why are they not being used (not even for thoroughly engineered lab and measurement devices where the small additional design effort could certainly be afforded)? Or is it relevant only for certain border-line cases?

Hatching was mostly about thermal relief and as others have said, keeping the copper load relatively even between PCB layers to reduce warping when the board heats up and cools down. With pumps and hoppers circulating the etchant around the boards, I would not worry about uniform etchant concentration.

You are not seeing hatched patterns much in modern equipment simply because PCB engineers had to learn to do away with them in modern high-speed electronics where hatching would wreck signal integrity on signals with sub-nanosecond rise/fall times.

[jakeypoo]

keeping the copper load relatively even between PCB layers to reduce warping when the board heats up and cools down

Give this man a prize.
If you have a solid plane on the top side, and mostly empty space on the bottom ( just a few traces ) the top will expand more during reflow and the PCB will be pringle shaped. There is a chance that it can cool that way and you end up with a non-planar pcb, which can make mounting less fun.

[poorchava]

This comes in handy for homemade PCBs fabricated with positive UV and toner transfer processes when your printer doesn't apply enough toner. Toner simply moves from the windows in the hatched pattern to the tracks making them thicker, which results in good, black solid hatched polygon rather then semi-oaque (or semi-covered) solid polygon.

[tautech]

This comes in handy for homemade PCBs fabricated with positive UV and toner transfer processes when your printer doesn't apply enough toner. Toner simply moves from the windows in the hatched pattern to the tracks making them thicker, which results in good, black solid hatched polygon rather then semi-oaque (or semi-covered) solid polygon.

Good tip thanks. 

[sfiber]

There is one reason to use pcb polygon,it's make pcb more beatiful but
if you dont mask pcb,soldering smd will be hard.

[salbayeng]

I'm with NandBlog & TerraHertz ,
In the old days, pcbs were made with a thick layer of copper, and it was necessary to etch through the full thickness , consequently you needed to hatch in the fill areas , and also avoid thin tracks running across bare PCB , both ensure a uniform etch and uniform undercut. 
Modern day PCBs start with a few microns of copper,  and plate up the rest of the thickness so it's really not necessary from that perspective.

And to control warpage you need roughly the same mass of copper on the top as the bottom, and hatching on the bottom (and the top fills) will provide the same average density all over.

I hatch all my fills (10mil track, 20mil pitch), it shows you have put a bit of thought into the PCB design.

[Precipice]

I hatch all my fills (10mil track, 20mil pitch), it shows you have put a bit of thought into the PCB design.

I have tier-1 manufacturers who ask (politely) that I use solid fills...
(I was saving weight, so used crosshatch for once - solid stitched copper is my default, has been for years).

[Dave]

keeping the copper load relatively even between PCB layers to reduce warping

I've learned that the hard way.
Here is a photo of a DIY PCB I made a couple of years ago.
It's about 20x10cm in size, bottom layer has a solid copper pour, while the top side barely has any copper on it. Both layers were tinned after etching. This is the result.

[T3sl4co1l]

Another good reason for solid is, RF leakage from inner layers (if applicable).

Tim

[salbayeng]

@Dave.
Nice pringle.

I see on your desktop you have one of those "radio shack key-chain pocket knives with wire strippers",  brilliant aren't they?

Do you ever accidently inject yourself in the wrist with the flux bottle? I keep mine on a shelf to avoid that possibility , also try a 28g tip on the flux bottle, gives a nice drop by drop control.

[Dave]

It's a Leatherman Squirt E4. Quite a handy tool.

I haven't managed to injure myself on those bottles. Yet.