1. Home
  2. Electronics Design
  3. DRC and split planes

DRC and split planes

Hi All,

I am using Protel PCB 2.8.

Yes it is ancient (1995) but it works, does all I need, and I know how to use it :) Also I often need to revisit very old projects - anything up to 20 years old. It runs fine in a winXP VM (VMWARE). I also have Protel 99SE which opens the v2.8 files apparently ok but so far have not felt the need to use it. I even found out how to generate gerbers for JLCPCB, who famously state they cannot read English and never read instructions on the layers, and who want apertures embedded within the gerber files.

However v2.8 can sometimes generate a lot of mysterious DRC errors. Some of these I have not solved and just leave them. Some are e.g. vias within SMT pads; it doesn't like that.

But others relate to "broken nets" where a plane has been split with a track, to get correct grounding routes etc. I don't like to ignore DRC errors; it is like ignoring compiler warnings.

Protel PCB requires any such breaks to be done with a polygon (a specific feature), not with just a normal track. But even when I do this correctly, it still reports some plane segments are being unconnected. This appears to be related to splits which have tracks at an angle, not 90 degrees, leading me to suspect that they use some sort of geometric algorithm to work out the connection topology and this breaks with polygons which have say 45 degree tracks. The user manual is silent on this.

OTOH I would have thought that algorithms for working out if you are "inside" a shape, for any arbitrary shape, have been thoroughly worked out in the 1960s, so why these issues in the 1990s?

I wonder if any modern PCB software does this sort of thing absolutely correctly?

Reply to
Peter
Loading thread data ...

In PADS, if you run vias or traces inside a copper plane area, it just provides the required clearances. Of course, that slices up the nice copper pour, which is your choice. If you absolutely break the power pour, it properly throws a connectivity error.

--

John Larkin      Highland Technology, Inc 

The best designs are necessarily accidental.
Reply to
jlarkin

You may have to recheck for artifacts with missing net assignments - corners that are strangled, underlying traces etc.

Do you examine printouts of the gerbers closely? These may show problems that are not obvious on the PC screen's GUI.

RL

Reply to
legg

I'd suggest getting used to Protel 99 SE (make sure you have SP6 which fixes a bunch of problems.) I can say the design rule check on P99 SE with SP6 is flawless. I have probably done 500 different designs with it, and have never felt the need to upgrade.

It also generated RS274X gerber files with the embedded apertures, and even if you design in inches, it can export the gerber and drill files perfectly in metric.

I've been running P99 SE under a VM for many years, first under VMWare (their software is excellent, but their phone support is the worst I have EVER experienced) and now under VirtualBox (never needed any support).

Jon

Reply to
Jon Elson

I used 2.8 for years until I retired. Had the same problem with 'power pours'. Sometimes there would be and Isolated pour and therefore an unconnected net. All I used to do was to link them both with a meaty track on the opposite layer ( mostly). Job done.Sometimes, I adjusted tracks so the pour WOULD connect. Having said that, all of my boards were fairly simple double sided jobs.

--
This email has been checked for viruses by Avast antivirus software. 
https://www.avast.com/antivirus
Reply to
TTman

snipped-for-privacy@highlandsniptechnology.com wrote

Does that work regardless of the shapes or tracks you put in the plane(s)?

Reply to
Peter

legg wrote

Yes; the gerbers are absolutely fine.

Reply to
Peter

Jon Elson wrote

Does 99SE say anything about

- needing a *polygon* for correctly breaking any planes?

- restrictions on angles of the polygon tracks?

I found v2.8 does actually do that too. Took me a while :)

I use VMWARE fr the winXP VM and have never needed support, although some obscure things don't work under it. Protel 2.8, 99SE and Orcad SDT386 all work fine.

I ought to probably try the DRC in 99SE - even if I just use 99SE for the DRC and nothing else. It does seem to open v2.8 .pcb files correctly.

Reply to
Peter

Yes. It maintains whatever clearance you want around anything, trace or pad or shape, that's a different net from the pour.

formatting link

It can even automatically resolve pour overlap conflicts, but I prefer to draw the pours exactly the way I want them.

That's a "copper pour" in the pic. There is also "copper", which paves over anything. Both are drawn "shapes" with net names and some rules.

PADS also has split/mixed planes and "plane connect" areas, neither of which I understand or like.

--

John Larkin      Highland Technology, Inc 

The best designs are necessarily accidental.
Reply to
jlarkin

The only restriction I know of is that a split-plane region may not be completely enclosed within ANOTHER split-plane region. But, a split plane region may be completely enclosed within a power plane. That pretty much relieves this as an obstacle.

power planes and split planes are NOT the same as pours, and are drawn in negative sense.

Yes, I think pours can only have horizontal/vertical tracks or 45 degree tracks. I rarely use the pours, mostly use power and split planes.

Jon

Reply to
Jon Elson

That's good, although I notice you are using only 90 degree angles :)

The algorithm is more complicated for an arbitrary polygon.

Signals within planes can be useful, although when I had tracks within planes I have always put the tracks on another *signal* layer, and put a thick track in the plane to exclude the copper from it, and then put a note on that signal layer to merge that with the said plane. The problem: the PCB fab needs to read English, which JCLPCB specifically state they never do; they never read any notes, so the gerbers needs to be supplied "finished". I guess most gerber editors can merge layers and re-output them.

I use split planes often, to create separate bits of GND, avoiding voltage drops etc.

Plane connect; no idea what that does.

Reply to
Peter

Most people use diagonal routing, multiples of 45 degrees. When I do fast stuff, I do direct (AA, any angle) routing to keep fast traces short, with minimal numbers of corners. That annoys some people; too bad.

People also like to worry about right angles, acute angles, acid traps, paving entire layers, silly things like that. Don't get me started on teardrops.

PADS handles pour clearances perfectly in all cases, as far as I know. It sometimes does strange things with thermals and net names. It won't do an inner pour unless you explicitely route into it with a via, which I guess is on purpose.

I need a PCB layout program that lets me do anything I want on any layer. I want to make the rules.

Some of the cheap quick-turn board houses just don't read fab notes. The resulting stackups can be bizarre.

formatting link

I don't either. It's like a copper pour but more complex and not well explained.

Nobody has ever explained to me what a split/mixed layer does, so I don't use them.

--

John Larkin      Highland Technology, Inc 

The best designs are necessarily accidental.
Reply to
jlarkin

torsdag den 7. januar 2021 kl. 18.42.23 UTC+1 skrev snipped-for-privacy@highlandsniptechnology.com:

so don't use planes, make all the layers signal and use pours ?

afaict planes done in inverse is just a leftover from when pcbs were done with tape and film and it was easier to do a reverse of the pads than cover everything with tape

Reply to
Lasse Langwadt Christensen

Right. Works fine.

I remember tape on mylar, rubylith and x-acto knives, and sending stuff to fancy photographers to get film.

Don't miss any of that.

--

John Larkin      Highland Technology, Inc 

The best designs are necessarily accidental.
Reply to
jlarkin

But... I want to. I've seen it recommended, but would like to hear a cogent argument for and against.

CH

Reply to
Clifford Heath

Oh, you want a *cogent* argument? Good luck. I've dug around and never fo und much basis for this. Some sources (sources that are not much better th an the guys at the water cooler) say acid trapping is what tear drops are a bout. Some say it is a matter of mechanical stability preventing breaks at the joint of trace to pad/via ring. Some say it is about preventing the t race from being cut off when the drill wanders off center (seems it is allo wed in IPC class II, not sure about class III) breaking the edge of the pad . When at the point of entry of the trace the trace can be cut, the tear d rop prevents this until the amount of wander is *much* greater.

So take your pick. Do tear drops solve a problem with acid traps (is there a problem to solve)? Do tear drops solve a problem of traces cracking at the pad/via? Do tear drops solve a problem of drill wander cutting traces from the via? Or is it all three? Don't know.

While researching this I found mention that tear drops were required for hi gh reliability equipment such as medical and aerospace. Anyone know about that?

--

Rick C. 

- Get 1,000 miles of free Supercharging 
- Tesla referral code - https://ts.la/richard11209
Reply to
Rick C

Silly. Ugly. Useless.

Reply to
John Larkin

Teardrops are useful on single sided boards with unplated holes. They help to provide slightly greater area for copper adhesion and help relieve peeloff and cracking from stress and vibration on the component lead. On modern through hole plated boards they are not needed as the hole plating anchors the component lead more strongly. I don't know of any reasons against having teardrops.

piglet

Reply to
piglet

Long ago, when I designed a circuit and PCB for the IRAS satellite it was mandatory to use teardrops for all connections. Also, bends in traces were required instead of angles. All for mechanical stability in a challenging temperature varying environment. For railroad work teardrops were (are?) required for pads of all 'heavy' components and connectors. I've always kept that rule in all my designs, it prevents cracking on the transition from pad to trace. Do not assume mechanically loaded PCB material is rigid! I've seen pads separated from traces to connectors where vibrating cables were flexing the connector.

Arie de Muijnck

Reply to
Arie de Muynck

I haven't done any ss boards since I was a kid. Pads without plated holes are positively eager to jump off a board. Single-sided layouts are mostly useless. We rarely even do double-sided boards any more; 4 layers is our minimum. They are cheap nowadays.

I've never seen a trace crack where it enters a pad with a proper plated-through hole.

They

Because they take time and are ugly?

They also complicate picosecond design, especially going into connector pins where the cad software will generate enormous teardrops.

Teardrops and acid traps and curvy traces are ancient legends that no longer make sense.

Reply to
John Larkin

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.