Jump to content
Due to a large amount of spamers, accounts will now have to be approved by the Admins so please be patient. ×
IGNORED

PCB Design - Advice RE copper pour


Recommended Posts

After some advice regarding using a copper pour in a PCB design.

 

My belief is that I can use a copper pour to:

 

1. Create a stronger ground, prevent ground loops.

 

2. More easily connect all required components to ground, rather than routing a string of traces everywhere.

 

3. Provide some shielding for video/audio lines.

 

Are these suitable reasons for utilising a copper pour?

 

Am I able to simply create a copper area that encompasses a majority of the PCB, attach it to the ground net and be done with it, meaning all other components with a pin attached to the ground net will have a ground connection to the copper area without needing to route individual traces?

 

Am I thinking about this along the right lines or am I way off? Educate me!

Link to comment
Share on other sites

Not sure if there's a distinction between the terms 'copper pour' and 'ground plane' either, and if it's software dependant.

 

Maybe the term ground plane better describes my situation. I'm using FreePCB which uses 'copper areas'. I've drawn out a copper area and attached it the the ground net. It appears to be doing what I seek, the gerber file output shows what I believe is correct. Wondering if there's any reason to be cautious about using a large copper area that serves as ground, will I encounter too much resistance with so much copper dedicated to ground?

Link to comment
Share on other sites

Thanks!

 

After reading through the documentation of FreePCB I believe the copper area is working as intended.

 

I've drawn out a copper area, and shaped it so that it covers all required ground points, and attached it to the ground net. It automatically creates thermal reliefs. The copper area is on the bottom layer, so for pads that don't have a hole and are only present on the top layer, I've created a stub trace that ends with a via. This connects the component to the ground plane.

 

Initially I had the copper area covering the entire board but thought this may not be optimal, so have resized and shaped it to only cover the areas needed.

 

I hope I've done it correctly and that it works, so much easier creating a common ground plane rather than running traces everywhere.

Link to comment
Share on other sites

All sounds like you have got it correct.

 

I usually first size the outline of the board then make the copper area as you have with some edge clearance.

 

After that, as you place each part, simply right click the grounded leg (if the part has one) and specify "ground" or whatever you have called the copper area in the dropdown box and that leg will attach by itself.

 

Depending on how "busy" your board gets, be careful to check the output .png picture to make sure you haven't orphaned any of the grounded points BEFORE you order boards.

 

I always specify a wider "track to fill" distance as well because I don't want potential shorts because of the fill being too close to the tracks. That is done at the 'generate CAM files' stage.

 

Here is an example of one I failed to check correctly (always too rushed) and you can see the ground pin of the chip is actually not connected to the copper.....fail!! Lucky I only had 10 boards made and we will keep these as factory test boards.

 

969863505_ScreenHunter_645Feb_0415_20.jpg.fc056d724995dbdc070b660c2ef1595d.jpg

Link to comment
Share on other sites

Depending on how "busy" your board gets, be careful to check the output .png picture to make sure you haven't orphaned any of the grounded points BEFORE you order boards.

 

I always specify a wider "track to fill" distance as well because I don't want potential shorts because of the fill being too close to the tracks. That is done at the 'generate CAM files' stage.

 

Here is an example of one I failed to check correctly (always too rushed) and you can see the ground pin of the chip is actually not connected to the copper.....fail!! Lucky I only had 10 boards made and we will keep these as factory test boards.

 

[ATTACH=CONFIG]123566[/ATTACH]

 

You've just stumbled upon my next question! My board is very busy and after viewing the gerber file output, I noticed a couple of pads with no connection to the copper area. Doesn't appear to be much I can do about this without a major redesign. :(

 

Does it generally matter which layer (top/bottom) the ground copper is placed? Any harm in having a large copper area on both top and bottom layers?

Link to comment
Share on other sites

Bottom is usually best because sometimes component legs fit through the hole at an angle and can short on the copper if it is on the top and the clearance is close.

 

My problem in the pic above was easily fixed by moving the vias to allow the copper to pour through BUT I could also have added a track to the top of the board connecting two earth pins together to achieve the same thing.

Link to comment
Share on other sites

What layer you use for the polygon (ground plane) will depend on if you use surface mount or through hole parts, as well as other factors. Sometimes I use polygons on both layers to get enough overall coverage or current capability.

 

What I do these days (in Altium) is turn on single layer mode after I've poured the polygons. Stepping through the layers in that mode gives you a much clearer idea of how complete the polygon is. Sometimes moving the odd track here and there (or to the other layer) can make a huge difference to how continuous the polygon is.

 

@Homepin how did that board pass DRC ?

Link to comment
Share on other sites

What layer you use for the polygon (ground plane) will depend on if you use surface mount or through hole parts, as well as other factors. Sometimes I use polygons on both layers to get enough overall coverage or current capability.

 

What I do these days (in Altium) is turn on single layer mode after I've poured the polygons. Stepping through the layers in that mode gives you a much clearer idea of how complete the polygon is. Sometimes moving the odd track here and there (or to the other layer) can make a huge difference to how continuous the polygon is.

 

@Homepin how did that board pass DRC ?

 

It didn't - problem is I was pushed and too rushed to run any tests - I just sent them out and had 10 made :redface

Link to comment
Share on other sites

The DRC in FreePCB doesn't seem to pick up on errors like that, where pins are isolated from the copper area by traces etc. It will tell you if a pin isn't covered by the copper area, but not if it's 'trapped' out of the copper area.

 

- - - Updated - - -

 

That rectangular pad on bottom left has no way of reaching the copper area? I thought I was being so clever and neat with my routing, seems I may have stuffed myself up.

20180203_220038.thumb.jpg.3383448e215946cb137d3e588be20a92.jpg

Link to comment
Share on other sites

If you find yourself having trouble getting things connected / grounded, it can be a sign of sub optimal parts placement.

 

Moving things around can change "routability" considerably. Does the D15 connector need to be on that side of the board?

Link to comment
Share on other sites

I think I'm grounded, barring far left bottom rectangular pad.

 

You need to redesign.

 

Connectors should be moved to give minimum trace length - And you have those traces running about as long as you could make them if you were trying.

 

 

 

[Added]

Another way of gaining useful experience when starting out is to design it in another software package.

A lot of design terms and techniques become apparent when presented from another packages point of view.

 

I'd recommend Kicad - Because there are plenty of Tutorials - From introductions to advanced techniques.

Link to comment
Share on other sites

I think it's ok.

 

Both DB15s need to be where they are. They are just joystick inputs so no major current flow.

 

I put the emphasis on making the power/video/audio traces as thick and as short as possible. These are my priority as thickness and length of trace does make a difference, whereas the controller inputs are a very low voltage signal. I'd rather route the less critical controller inputs out of the way and prioritise real estate for power, audio and video.

 

- - - Updated - - -

 

I do have Kicad however cannot use it much due to its internet dependence (still waiting for NBN and no wifi in my area). I also have PCB Elegance which I quite like.

 

I do see the importance of what you are saying, I just don't think it pratical to keep every trace as short as possible, and if allowances have to be made I think the controller inputs are the best connections to 'sacrifice'. I think of a typical arcade cab that has meters of wiring with joysticks and buttons connected by very thin/cheap wiring using quick connects...

 

In testing the prototype behaves perfectly. I've tested it against two other superguns (Vogatek and Mak Strike) and my supergun is the only one that syncs all arcade game boards on all my test monitors (Sony PVM, Sony BVM, Philips CRT TV, Bang & Olugsen CRT TV, Commodore 1084) without any signs of video interference. It is the only one with clean, non-distorted audio. Additonally, my design only utilises 28 vias whereas the Vogatek is close to 100 and Mak Strike well over 100. Finally, my power traces are considerably thicker and shorter than both.

Link to comment
Share on other sites

You need to redesign.

 

Connectors should be moved to give minimum trace length - And you have those traces running about as long as you could make them if you were trying.

 

 

 

[Added]

Another way of gaining useful experience when starting out is to design it in another software package.

A lot of design terms and techniques become apparent when presented from another packages point of view.

 

I'd recommend Kicad - Because there are plenty of Tutorials - From introductions to advanced techniques.

 

I made a note earlier in this (or maybe it was a different but similar thread?) about choosing the program you use carefully if you want "outside board houses" to make your boards.

 

I can assure people that "all gerber files ARE NOT created equal" and there are many board houses that are becoming fussier as the price drops. I have not had a single board factory knock me back supplying files from FreePCB or Altium but I did try and have some boards made for a customer one time, supplied to me in Eagle and both of the main board factories I deal with simply said "no".

 

I'm unsure about Kicad but, from memory, it's basically an in-house "you must use our service" kind of thing and that is bad news in the long run because it 'can' cause issues when you try to get boards made by someone else.

 

I'm sure there are many other programs that work fine and are acceptable to board places but we stick with FreePCB and Altium. Actually practically all of the boards in our pinball are made using FreePCB - it's fast, easy to learn, accepted by all places we have used and very stable PLUS - it's FREE :lol It has some drawbacks and when we strike thise we use Altium but it is very top heavy with a very steep learning curve.

Link to comment
Share on other sites

I've been extremely happy with FreePCB! The only feature so far that I have needed that isn't present is routed slots. E.g. the ability to create a square or rectangular hole. The option is present in the drop down menu but it's grayed out, not sure if it's a feature that was never fully implemented or if I just don't know how to access it.

 

Some people have expressed disappointment with its lack of an auto-router, however there is one available that plugs straight in - freeroute. I actually don't like using it though, it only really excells with simple designs (may as well just route by hand) and I find the human touch is always better. Sometimes I use it just to get an idea of the best/shortest paths but predominantly I route by hand.

 

- - - Updated - - -

@Homepin With FreePCB, if I draw a board outline within a board outline, does that create a cutout/hole? I.e. a 50mm x 50mm board outline with say a 10mm x 10mm outline drawn in the middle, would that create a square PCB with a small square hole in the middle?

Link to comment
Share on other sites

I've been extremely happy with FreePCB! The only feature so far that I have needed that isn't present is routed slots. E.g. the ability to create a square or rectangular hole. The option is present in the drop down menu but it's grayed out, not sure if it's a feature that was never fully implemented or if I just don't know how to access it.

 

Some people have expressed disappointment with its lack of an auto-router, however there is one available that plugs straight in - freeroute. I actually don't like using it though, it only really excells with simple designs (may as well just route by hand) and I find the human touch is always better. Sometimes I use it just to get an idea of the best/shortest paths but predominantly I route by hand.

 

You can easily make routed slots as long as they have straight sides (any shape). FreePCB won't do curved slots or board edges though. I also much prefer hand routing - much better control over placement etc.

 

Here is a board with a cutout in the middle made with FreePCB:

 

stepper1.jpg.2db8d9c44a5a81a66eb911e68b8e2275.jpg

 

stepper3.thumb.jpg.7d6b2acd935bac97f4318d3b6bfc25d1.jpg

 

Just use "ADD > BOARD OUTLINE" and make your shape anywhere you like - the gerbers will show a cutout in your made shape.

 

Here are a few quick examples I just hashed up in 30 seconds:

 

689886774_ScreenHunter_646Feb_0508_32.jpg.ef77e4e07b4c2455da0843bd3118a105.jpg

Link to comment
Share on other sites

Impeccable timing Homepin, I just updated my post asking the very same question!

 

You can indeed do rounded edges Mike, create a board outline and select an edge, right click to insert and position a corner, right click the edge and select 'convert to arc'.

Link to comment
Share on other sites

Impeccable timing Homepin, I just updated my post asking the very same question!

 

You can indeed do rounded edges Mike, create a board outline and select an edge, right click to insert and position a corner, right click the edge and select 'convert to arc'.

 

Well that's news to me...thanks very much.

 

Based on your idea, I guess you can also apply this to rounded slots and cut outs? I'll give it a go later when I get a chance.

 

Based on this, we will be using Altium even less now :lol

Link to comment
Share on other sites

Here's a quick and dirty demo.

 

Look at the picture I've attached:

 

Top left corner shows two inserted corners, both 2mm out from the main corner. Select the main corner and 'move' it inwards by 1mm. This creates the angled corner as shown. In fact this process is over complicated, just create an angled corner to begin with! I've done it this way to show you the full possibilities.

 

Bottom right corner shows - selecting each of the 2 segments of the angled corner, right clicking and selecting 'Convert to Arc (ccw)'. Select and delete the corner in the middle to end up with a rounded edge as shown in the top right corner. If you just draw a board outline with an angled edge this last step isn't necessary, but doing it this way illustrates further possibilities.

 

Have also drawn a funny shape in the middle.

 

Exact same technique can be applied to polylines when creating footprints.

freepcb_outline.thumb.png.dde6792c8e3c1c61974de4b28178a8a2.png

Link to comment
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now
  • Recently Browsing   0 members

    • No registered users viewing this page.
×
×
  • Create New...