How to avoid very thin lines appears in the pour copper ?

[Boncuk]

In addtion, curve is useful. I believe that it would be better if electrons run in a smooth curve.

View attachment 61911

Nice knitting pattern and one more face.

Eagle has a good function called "ratsnest".

When placing unrouted components they are connected using "air wires". Move parts around until the air wires are reduced to the least amount of crossings. Perform ratsnest after each movement.

Boncuk

 

[jpanhalt]

In addtion, curve is useful. I believe that it would be better if electrons run in a smooth curve.

I hope you are not serious with that comment from a electronic sense. Aesthetically that may be what you like, but since you are a major PCB manufacturer, you should follow the most recent version of IPC-2221.

Here are some other sources you might find interesting:

1) https://faculty.yu.edu.jo/myhomari/default.aspx?pg=c94d397c-06fd-4dfc-a4d5-7d5c25eccb06

Section 5.3.2

2) https://www.electro-tech-online.com/custompdfs/2012/03/PCBDesignTutorialRevA-7.pdf (do not click on the link for a more recent version)

David L. Jones
PCB Design Tutorial
Page 11/25

Tracks should only have angles of 45 degrees. Avoid the use of right angles, and under no circumstances use an angle greater than 90 degrees. This is important to give a professional and neat appearance to your board. PCB packages will have a mode to enforce 45 degree movements, make use of it. There should never be a need to turn it off. Contrary to popular belief, sharp right angle corners on tracks don’t produce measurable EMI or other problems. The reasons to avoid right angles are much
simpler - it just doesn’t look good, and it may have some manufacturing implications.

Forget nice rounded track corners, they are harder and slower to place and have no real advantage.
Stick to 45 degree increments. Rounded track bends belong to the pre-CAD taped artwork era.

Regards, John

 

[PCBWING]

I hope you are not serious with that comment from a electronic sense. Aesthetically that may be what you like, but since you are a major PCB manufacturer, you should follow the most recent version of IPC-2221.

Here are some other sources you might find interesting:

1) https://faculty.yu.edu.jo/myhomari/default.aspx?pg=c94d397c-06fd-4dfc-a4d5-7d5c25eccb06

Section 5.3.2

2) https://www.electro-tech-online.com/custompdfs/2012/03/PCBDesignTutorialRevA-1.pdf (do not click on the link for a more recent version)

David L. Jones
PCB Design Tutorial
Page 11/25


Regards, John

Thanks. Those are good books. But I‘m not sure if the expositions of the rounded track has actual measurement data to support. I will ask Dave about that. Maybe he would let me know why or maybe he would change his mind.

 

[PCBWING]

Nice knitting pattern and one more face.

Eagle has a good function called "ratsnest".

When placing unrouted components they are connected using "air wires". Move parts around until the air wires are reduced to the least amount of crossings. Perform ratsnest after each movement.

Boncuk

Thanks. In fact, I am not familiar with the Eagle. But I know it is a household name for the Electronic engineers.

 

[Jugurtha]

Hello,

Learn Eagle. Read the whole manual not to ask how to do things, draw boards and post pictures to ask how to do things "better" from experienced users.

Here's my first thread about Eagle: (I had read the manual and tried my best to do a board, then commented every step and why I did it so an experienced member would spot any wrong mind-set (example on avoiding the traces beneath the uController to avoid interference, which got corrected by Ronsimpson. I wouldn't know this wasn't important had I not formulated my thoughts explicitely. On moving lines too.)

https://www.electro-tech-online.com...th-cadsoft-eagle-critique-appreciated.122577/

I got a tremendous help from Boncuk who took the time to show me what a beautiful board was and I got inspired.

Then, I drew another board and tried to follow guidelines (notamment from Dave Jones PDF). And each time I got a revision, I would log in the Chat and had people give me feedback on my boards (Were the lines too thin ? Where they too close ? How would they do it better ?) .. And get back to work with their remarks. (3v0, Jon_Wilder, Inquisitive, Hayato, DerStrom8, Microman, etc ...) Then actually print the board and have a PCB. Inspect it and see problems that don't really appear on the screen. (like pads too small so that when you drill, you break contact, you actually eat the copper).


Here's for example an attached PDF of a recent board. This is the twentieth version or more. Each time you change something. (In this one, I had to manually change the pads size in the libraries, one by one (must learn to script) ).

See how ugly was the beginning ? Still, the board isn't perfect, but for the size and the tools I have, it does the job.

 

[unclejed613]

In addtion, curve is useful. I believe that it would be better if electrons run in a smooth curve.

View attachment 61911

actually since (unlike water) electrons have very low mass, it makes no difference what the corner looks like.

 

[phalanx]

The piece of copper on the right between the three pads and the trace is not connected to anything so it should not be there.

In Eagle, that piece of unconnected copper is called an orphan. There is a setting you can apply to your polygon that will either leave them in like your current board, or remove them completely.

 

[ronsimpson]

actually since (unlike water) electrons have very low mass, it makes no difference what the corner looks like.

And unlike water electrons move pretty fast.
At RF and where reflections are a problem, corners are a problem. Many PCB manuals say not making 90° angles because of etching undercutting. They like two 45° angles. Many people rally avoid greater then 90° angles.

The "spaghetti" layout above reminds me of when we used to do layouts by hand with red and blue tape, (black flexible tape). I have not seen much of that in modern history.

 

[PCBWING]

Jugurtha, I think it is good.

 

[PCBWING]

unclejed613 , I thought it may be on the contrary, high-speed might make it to need more smooth rails. It is only my guess of course.

 

[PCBWING]

And unlike water electrons move pretty fast.
At RF and where reflections are a problem, corners are a problem. Many PCB manuals say not making 90° angles because of etching undercutting. They like two 45° angles. Many people rally avoid greater then 90° angles.

The "spaghetti" layout above reminds me of when we used to do layouts by hand with red and blue tape, (black flexible tape). I have not seen much of that in modern history.

Yes, I remember that. But now some of the CAD software can support the curve.

 

[PCBWING]

Raster or Vector

If that comment is in response to my comment immediately above, then NO, I am not talking about the cross-hatch or lines fill (not available on Eagle) options. If you think of the fill as a vector rather than bit map, the fill is with lines that touch. The thicker the line, the more jagged will the edges be. The thinner the line, the more processing it takes. Eagle used to have a warning to that effect. Line width does not affect the gross appearance of the filled areas in Eagle, unless you pick the cross-hatch option.

Just to clarify, there are multiple ways to do what you asked in your first post. Your later post on page 2 illustrates one of the problems of using isolate as the variable. Of course, you can avoid that by using multiple polygons. The restrict method avoids that too, and I find it easier to do in a controlled and precise manner. In Eagle, isolate and line width can affect other things too, like the the way thermals are made.

Finally, as to the patch of copper that is not connected to anything, that is called an "orphan" in Eagle. You can choose to have them left in place or removed.

BTW, Are you actually a PCB manufacturer or is that just an avatar you like?

John

I did a test. The vector sample would export a larger size Gerber than the raster sample.
I attached the images of it.
----------------------------------------------
Filename size date time
Raster.gbr 17,937 2012-03-29 11:22
Vector.gbr 67,088 2012-03-29 11:22
----------------------------------------------

View attachment 62761
View attachment 62762