Copper Pours + GND? - Page 1
Forum section: electronics / general

author: BloodyCactus
author_rank: Frequent Contributor
timestamp: May 07, 2014, 12:58:33 am
content: aaargh. So converting over from Eagle, so far everything is great except ONE thing that REALLY bothers me, attaching a copper pour to both sides of my board to GND, it still wants to route the gnd ratlines, even when connected to a pour. I ran the auto route to get an idea of how I might manually route, and it makes all these compromises because it routes all the GND lines..So I export a DSN to FreeRoute... copper pour does not come over attached as gnd, so FreeRoute routes all the GND lines. ugh.That and the copper pour don't update automatically. manually updating is irritating.Otherwise, all is good.

author: c4757p
author_rank: Super Contributor
timestamp: May 07, 2014, 01:23:04 am
content: Quote from: BloodyCactus on May 07, 2014, 12:58:33 amSo? The copper pour still has to get through the same places the traces would have to get through.

author: John Coloccia
author_rank: Super Contributor
timestamp: May 09, 2014, 09:27:59 am
content: Highlight the GND net with your mouse....just hover over a pad that's part of your net. Right click, and select Net Properties. Under Route Mode, select Don't Route. Voila'.But heavens, why are you using the auto router? Even the really good ones somewhat suck, and DipTrace isn't a really good one.

author: BloodyCactus
author_rank: Frequent Contributor
timestamp: May 09, 2014, 11:48:32 am
content: Telling it 'dont route' did not seem to apply when I tested it to the autorouteror to exported dsn file for freerouter. I use it sometimes to get a sense of how I should go about routing it.

author: John Coloccia
author_rank: Super Contributor
timestamp: May 09, 2014, 12:39:16 pm
content: I tried it before I posted. When you tell the net don't route, the autorrouter ignores it.

author: BloodyCactus
author_rank: Frequent Contributor
timestamp: May 09, 2014, 03:33:58 pm
content: hmm I wonder if its not a bug then, I ran into an issue where it should also not draw the air wires if its connected to the copper pour but did have air wires.

author: Mechatrommer
author_rank: Super Contributor
timestamp: May 09, 2014, 04:03:34 pm
content: hide GND net, avoid autorouter, do manual route, DRC ok, all is good albeit annoying sometime.

author: John Coloccia
author_rank: Super Contributor
timestamp: May 09, 2014, 04:16:28 pm
content: Quote from: BloodyCactus on May 09, 2014, 03:33:58 pmDefinitely sounds like it might be a bug in your version. I'm version 2.3.1. I just tried it again on a "real" design, and it did the right thing, just like it normally does. It routed everything but the ground and the ratlines disappeared. If you right click on a pad on the net, you can select "hide rat lines" and it will do that too. I usually hide the ratlines for my ground so that they're not bugging me when I do the routing. There's also an option in the copper pour for "Hide Rat Lines". It's selected by default. After the pour, it will hide the ratlines for that net.Are you sure you're selecting the Net you want under "Connectivity" in the copper pour? It won't automatically just connect to the "GND" net. You need to tell it what you want. In fact, if you wanted to you can do multiple copper pours on different sections of the board, and attach them to different nets.

author: DerekG
author_rank: Frequent Contributor
timestamp: February 07, 2015, 01:27:25 am
content: Quote from: John Coloccia on May 09, 2014, 04:16:28 pmEveryone does things differently & I'm interested in your method. I usually route the ground net first & then the power net(s). This means I'm doing the manual routing of nets in reverse to yourself.So, can you please further explain what you like about routing your other nets before your ground net?I'm certainly not criticising you in any way, just wanting to more understand your methodology.

author: John Coloccia
author_rank: Super Contributor
timestamp: February 14, 2015, 01:06:31 pm
content: My copper pour IS my ground, so I don't do anything with ground at all. I route everything else, and then the very last step is I do the copper pour. Unless I've done something REALLY crazy, that picks up all of my grounds.

author: DerekG
author_rank: Frequent Contributor
timestamp: February 15, 2015, 02:17:16 am
content: Quote from: John Coloccia on February 14, 2015, 01:06:31 pmGreat Idea. I've designed & layed out hundreds of boards & never thought of doing it that way. My tightly packed SMD boards often don't have a ground plane on the top layer, but I'll give it a go & see how it pans out.

author: Dave Turner
author_rank: Frequent Contributor
timestamp: February 15, 2015, 05:36:39 pm
content: I'm sure that I read somewhere that you should explicitly route the ground netlist before flood filling. Admittedly that might have been due to limitations of a particular CAD package as I've looked at several of the freeware packages.Is there any advice on this?

author: John Coloccia
author_rank: Super Contributor
timestamp: February 18, 2015, 10:15:39 pm
content: Quote from: Dave Turner on February 15, 2015, 05:36:39 pmIf you do that, it will completely defeat the purpose of the thermal relief on the pads. Perhaps there's some thought that you MAY want to try and route by hand as you go along to make sure that it's actually possible to connect everything with a copper pour. After all, if you can't get there with lots of little traces, you can't get there with a couple of monstrous traces either. I usually don't worry about it. If I end up with a broken net at the end, it usually just takes a few minutes to move the offending traces to fix it.That said, it's helpful that I spend a lot of time upfront working on my basic layout, and I identify problems early and try to mitigate them. If you just slap stuff on a board, hit auto route, and then hit the copper pour, there's a good chance you won't end up with something that works. Personally, I never use the auto router...ever...on any package, and I end up with boards that are mostly routed on one side, with occasional traces on the back side in trouble areas. These never give me a problem.

author: Dave Turner
author_rank: Frequent Contributor
timestamp: February 18, 2015, 11:08:41 pm
content: John ColocciaI made no comment about autorouters, neither did I mention thermal relief.I'm the veriest beginner when it comes designing a board but would still not rely on autorouting (though I do autoroute to see what comes out) as I'm trying to practise routing for fun/entertainment & hobbyist purposes.My previous experience was with letraset and tape.The observation made was simply that I had read somewhere that one should explicitly route the Ground netlist, which may or may not include defining thermal relief pads, rather than rely on connectivity being provided by a flood fill.Perhaps this was a limitation of whichever program I was reading about at the time.I was simply trying to find out whether this was general advice or perhaps limited to a particular program.

author: John Coloccia
author_rank: Super Contributor
timestamp: February 18, 2015, 11:26:24 pm
content: Quote from: Dave Turner on February 18, 2015, 11:08:41 pmI was just trying to answer you, Dave. I think you took away some sort of indictment or condescension from my answer. I didn't intend any.

author: steve_w
author_rank: Regular Contributor
timestamp: February 18, 2015, 11:40:50 pm
content: Hey John,Can you explain a little about thermal relief and the ground flood fill connection?I like Dave T am a beginner and am interested in why.I just did my first board and used flood fill, I am not really concerned with thermal relief as my board is only for signals not power but would like to understand the practical aspects of board layout.regardssteve w

author: Dave Turner
author_rank: Frequent Contributor
timestamp: February 19, 2015, 12:09:38 am
content: JohnMust be be semantics I didn't/don't understand how your answer was relevant to my question. No offence taken or intended.

author: John Coloccia
author_rank: Super Contributor
timestamp: February 19, 2015, 12:10:05 am
content: Quote from: steve_w on February 18, 2015, 11:40:50 pmSure, it's simple. When you're soldering to something attached to a big chunk of copper, like a copper pour for example, you'll have some trouble pumping enough heat into the joint to make a good joint. Thermal reliefs are generally implemented as little spokes that come off the pad and attach to the pour. They limit the flow of heat to the big chunk of copper, and make for easier soldering.You can generally configure them for shape and size. After the pour, you do need to examine the board closely to make sure that all of the reliefs are actually adequate. It's not unusual to loose a spoke or two on some pads because of clearance to a nearby component. You also want to check that the pour itself has good continuity without getting too thin in areas. For example, sometimes you end up with sections of the pour being connected to each other with these thin, strands of copper. It can happen because of clearance to other components or traces, and you just need to give the board a little scan when you're done to make sure that you're happy with what you have.I usually size my spokes so that I can loose two of them on any pad and I'm still good. Soldering would be slightly easier if I sized them to be barely adequate, but it's easy enough as it is, and this way I don't have to chase down every last issue to get a working board.But that's just my own design philosophy. There are probably lots of different ways to do this, and they're probably all correct in their own way.

author: John Coloccia
author_rank: Super Contributor
timestamp: February 19, 2015, 12:18:36 am
content: Quote from: Dave Turner on February 19, 2015, 12:09:38 amThere are a number of different reasons for doing a pour. Sometimes, you're just trying to lay down copper to keep a board from warping. Other times, you use the pour as somewhat of a ground plane (or power....or whatever net you wish, really...but it's often ground). Now see my answer to Steve's question. If you intend to use the copper pour to connect your grounds, routing the grounds together first just puts extra copper on the pads at best, defeating the purpose of the thermal reliefs you almost always use, and at worst is just a complete waste of time if you then have to come back and remove the manually routed traces.But you don't HAVE to use a "copper pour" feature to get a copper pour. It's not uncommon to define copper polygons by hand, and to connect everything like that. The copper pour command is something like an auto-router. You have some control, but in the end you get what you get. If you do a good job with your layout, keeping the copper pour in mind, then the command works great and you're done. The point I was trying to make is if you just start connecting things willy nilly, then the copper pour can fail just as miserably as an auto router.

author: tautech
author_rank: Super Contributor
timestamp: February 19, 2015, 12:24:45 am
content: I'd also add that SMD trace neckdown will provide some thermal relief.

author: John Coloccia
author_rank: Super Contributor
timestamp: February 19, 2015, 12:58:45 am
content: OK, so here's an example of a copper pour connected to ground, just so everyone sees it. Notice that the pour goes around and isn't connected to most of the pads, but that it connects to SOME pads with "spokes". Those are the thermal reliefs. If I didn't use thermal reliefs, it would simply go right up to those pads, and would be very difficult to solder. I have very few traces on this side of the board, so just snapping the pour to the board outline and setting it loose gives me a good pour with no real problems.Notice also that there are a couple of spokes missing from a pad or two. You have the option of orienting the spokes at 90 degrees or 45 degrees. In this particular case, orienting at 45 degrees gives me the best connectivity, and the couple that are missing are completely inconsequential, both because they're oversized and because I happen to know what they're connected to.Hope this helps visualize it a little bit.

author: steve_w
author_rank: Regular Contributor
timestamp: February 19, 2015, 02:48:09 am
content: John,Thanks for the picture. Makes complete sense now. I didn't use thermal relief on the board I just did and I expect to have a job soldering in some of the components.I wont make that mistake again.regardsSteve W

author: Simon
author_rank: Unknown
timestamp: May 05, 2015, 05:30:35 pm
content: I had the same problem wanting to do a large number of copper pours due to the current carrying requirement of the board. I then found that the auto route is an utter disaster because it will mark all rat lines to the parts in the copper poor as not rooted when they most certainly are. The only other option is to route the board and allow it to go through the copper pours where it will create clearance and therefore disconnect and break them apart. I had long email conversations with Alex about this problem and he did not seem to see the problem and the only solution he could offer or rather answer was for me to bear in mind that they are a small company and don't have the resources to do a proper job so just chucked something together. It is unfortunate that the free route up will not accept the copper pours as it is a far superior route and I could never do better myself. People seem to provide their also routers on how fast they are the dip trace one out of the box is very fast and very awful. I think you can increase in the options the amount of routing sweeps it does to try and improve it but it's still very mechanical and looks nothing like the great job free route does. I even suggested that they incorporate the free route up software into their own package and that the author would probably be quite happy to negotiate with them but got no reply. So I am afraid that complicated routing in dip trace is not possible unless you do it yourself hopefully these things will be addressed in time.

author: DerekG
author_rank: Frequent Contributor
timestamp: May 05, 2015, 11:15:02 pm
content: Quote from: Simon on May 05, 2015, 05:30:35 pmConnect the copper pour to a net (ground in most cases), repour it & then update from your Schematic. This should remove the rats lines as DipTrace will now see the nets as connected.Yell out if you want me to go through the menu steps for you.

author: Simon
author_rank: Unknown
timestamp: May 06, 2015, 06:48:29 am
content: the problem there is that you have to set the copper pour as a keep out zone to stop other tracks from other nets cutting through it and cutting it up, this then stop tracks from even the same net as the copper pour, I've tried it all, the only way around was to lay some normal traces where the copper pours would go just to make it happy and put the copper pours on top then run the autorouter and hope that a track already through the middle of it stops other tracks, like I said I had long emails with alex on this and he had no solution other than to say they are a small company and still working on it.

author: DerekG
author_rank: Frequent Contributor
timestamp: May 06, 2015, 07:05:08 am
content: Yes, it is always best to lay down all the other nets before the copper ground (or any other) pour.To do this, you deselect the ground net before running the auto-router. All the ground rats lines will now disappear.Once all the other nets have been routed (by the auto-router then cleaned up manually by yourself), re-active the ground net (FILE, RENEW DESIGN FROM SCHEMATIC).All the ground rats lines will now reappear.Now lay down your polygon plane & choose to connect it to the ground net.Once you pour it, all the ground rats lines should disappear (as long as the ground pour is able to be connected within your design rules).I have found this to be the fastest method that produces good results.I used to lay down my power & earth nets first, but not anymore.ADDED: Using the above method means that you don't have to worry about any other tracks cutting up your earth plane during auto-routing. You have in effect "reversed the procedure".

author: Simon
author_rank: Unknown
timestamp: May 06, 2015, 08:35:01 am
content: Derek, your missing my point, I need the copper pours to carry large currents, they need to be there and they need to be where i want them not where diptrace has room for them later. If I need large supply traces etc it is far easier to do it as a net connected copper pour than to have to manually do the pour with thick traces and the headache that becomes. I just draw the specific shape I need to cover the area I need and include the component pads i need to. Copper pours are not just for decoration, they can be part of the layout.

author: DerekG
author_rank: Frequent Contributor
timestamp: May 06, 2015, 09:47:58 am
content: No worries.Also remember you can open up the solder mask so that when the board is wave soldered, the solder will add to the thickness of the tracks, thereby adding to the current carrying capabilities.On the top side of the board, you can also open up the solder mask & the paste stencil (in a grid pattern) to lay down extra solder paste over the tracks / copper pours. I often do this to add current carrying capabilities & for extra heat dissipation. An example (generated in DipTrace) is attached. The red layer shows the exposed copper (no solder mask) & the yellow/gold shows the solder paste "squares" that will be laid down on the top layer.2oz & 3oz copper is also the go for extra current capabilities.If you feel that you would like to try another CAD package, take a look at Proteus - the developers are in the UK just like youI like & use it a lot.I also use Altium, but it comes in 3rd as far as ease of use. I also dislike Altium the Company as I'm sure you have also read in some of my other posts.