EasyEDA are these 2 areas circled in white correctly connected?

Thread Starter

clangray

Joined Nov 4, 2018
261
For the posted circuit in the photo, are the 2 track ends completely connected to the two pads (circled in white) - there appears to be gaps. DRC says "exists incomplete connection" but no other errors.

forum pic.jpg
 

Jon Chandler

Joined Jun 12, 2008
1,048
Nope. They are not connected because the connector is rrotated 180° from where it should be according to the schematic. Notice the thin blue "air wires" – they show the expected connection points.


I don't believe the LED is properly connected either.

Click on and highlight one pad, then hit H on the keyboard. Everything connected in the schematic will be highlighted.

Hit H again to clear the highlighting.
 

Thread Starter

clangray

Joined Nov 4, 2018
261
Ok, I think I've got a "blue air wire" problem. The highlighted areas are occurring along the "blue air wires" and disallowing connections other than blue wire connections. How would I fix?

I can connect pad-to-pad but how do I delete some existing blue air wire lines?
 
Last edited:

Jon Chandler

Joined Jun 12, 2008
1,048
EasyEDA works very hard to prevent connections that don't agree with the schematic. The air wires show the points that should be connected according to the schematic.

You can highlight nets as I described above. All highlighted parts should be connected. EasyEDA won't allow you to connect two points not in accordance with the schematic.

It looks like you have the headers rotated 180° from where they should be (Hmmm. I think I said that too). YOU might not care which is pin 1 and which is pin 2 on the header, but EasyEDA does – it doesn't know that the ends are the same.

To rotate the connector on the board, click on it and press R twice to rotate it 180°.

Pin 1 on many components is designated by a square pad. I'd suggest in the circuit shown, the square pads of the connectors should be connected to the square pad of the LED to keep the polarity straight.
 

Thread Starter

clangray

Joined Nov 4, 2018
261
I'm going to remake the schematic making sure all connections are correct before converting to PCB. I thought I did but apparently not.


forum pic 2.jpg
Please see photo. Are the two in the photo the same? I remember you saying that they needed to be flipped: apologies. I thought the lines jutting out of the component pins for attaching to a DuPont style connector. That's what I need at least(right angle male header/ connector). The pins for connection need to be on board edge for access.

I guess cut and pasting components in between PCBs is not correct either.
 
Last edited:

Jon Chandler

Joined Jun 12, 2008
1,048
Here's a similar schematic to what you're doing, mirroring somewhat the board layout. When positioning the connectors, the pin numbers are important.... well, at least I'd keep the connections the same. Pin 1 connected to pin 1. One of the connectors is rotated 180 degrees compared to the other and I've shown where the pins are.

Junk3-0.jpg

It's equally valid to draw it without representing placement on the circuit board. In the version below, I flipped one of the connectors over to align pin 1 for a cleaner-looking schematic. The end result will be the same in either case.

junk3-0a.jpg

When you "convert to PCB", the components are dumped onto a bare canvas for the circuit board. The thin blue "air wires" show which pads are connected to which. Sometimes it can be difficult to tell what goes where - hitting H will show all the connections of the net.

junk3-1.jpg

From there, start to position the components as you like. Highlight each net to see where the connections go if need be. Notice that if the connectors are rotated with respect to each other, the pins don't align across the board.

junk3-2.jpg

Next, route the tracks. You can only connect pads as shown in the schematic (without editing). If a track won't connect to a pad, it's not supposed to be connected. You can connect the pads by a cirtuitious route, or you could take a more direct path on the bottom layer of the board.

junk3-3.jpg


I would still recommend each LED has its own series resistor rather than operating them on parallel. LEDs don't always share current gracefully, and by having independent current limiting resistors, you can add or subtract LEDs from the chain as desired.
 

Thread Starter

clangray

Joined Nov 4, 2018
261
Here's a similar schematic to what you're doing, mirroring somewhat the board layout. When positioning the connectors, the pin numbers are important.... well, at least I'd keep the connections the same. Pin 1 connected to pin 1. One of the connectors is rotated 180 degrees compared to the other and I've shown where the pins are.

View attachment 283663

It's equally valid to draw it without representing placement on the circuit board. In the version below, I flipped one of the connectors over to align pin 1 for a cleaner-looking schematic. The end result will be the same in either case.

View attachment 283664

When you "convert to PCB", the components are dumped onto a bare canvas for the circuit board. The thin blue "air wires" show which pads are connected to which. Sometimes it can be difficult to tell what goes where - hitting H will show all the connections of the net.

View attachment 283665

From there, start to position the components as you like. Highlight each net to see where the connections go if need be. Notice that if the connectors are rotated with respect to each other, the pins don't align across the board.

View attachment 283666

Next, route the tracks. You can only connect pads as shown in the schematic (without editing). If a track won't connect to a pad, it's not supposed to be connected. You can connect the pads by a cirtuitious route, or you could take a more direct path on the bottom layer of the board.

View attachment 283667


I would still recommend each LED has its own series resistor rather than operating them on parallel. LEDs don't always share current gracefully, and by having independent current limiting resistors, you can add or subtract LEDs from the chain as desired.
Thank you so much for that detailed guide! Very impressive thank you.
 

Thread Starter

clangray

Joined Nov 4, 2018
261
I've supplied the overall schematic. Isn't it in series? But you would also still recommend a resistor per connector?
I've rebuilt the PCB from the schematic following the same steps as you : I was sure to make the schematic correctly. It worked out great, DRC = 0. Just have to fix the pin issue and probably rebuild again. No more ratline issues because you fix them in the schematic before creating the PCB. The black box illustrates the "main" board with PS and ballast resistor. I've prototyped this with Adafruit tiny breadboards - works fine so far.

Oh, how do you flip a component? I know how to rotate. (got it! X or Y after component selection)
circuit (28).png
 

Attachments

Last edited:

Jon Chandler

Joined Jun 12, 2008
1,048
What you have will work. But there are a couple points to consider:

o You have to run a complete loop of wire back to the power board

o Failure of any of the LEDs extinguishes them all

o If you want to change the number of LED boards, you have to change the series resistor

o If you have different color LEDs, you can't adjust the individual currents to equalize brightness


I would accomplish this using parallel LED+resistor boards, with the resistors sized for the supply voltage. This addresses all of the above, and probably eliminates the need for the power board completely.

junk3-4.jpg

I don't know what you're trying to accomplish, so you may have your reasons for a series arrangement. My design philosophy is to usually take a wider view to think about simple changes that make things more flexible and useful for other applications.
 

Thread Starter

clangray

Joined Nov 4, 2018
261
That's really interesting parallel + resistor boards. Your points were taken. Let me contemplate.

Thanks for taking the time.
 

Thread Starter

clangray

Joined Nov 4, 2018
261
One last q: should I put the 8 connectors on 1 sheet? It seems your schematic has 4 of them. Do all 4 convert to PCB at the same time?
 

Thread Starter

clangray

Joined Nov 4, 2018
261
So I am uploading a schematic that is the parallel circuit above (post #14) but with an added power source. I added a barrel connector as PS. It still has connectors to pass power and ground to other connectors. And look, no main board. When I render it in EasyEDA it looks correct at least parts wise. Just wanted you to check electrical and see if correct:

Renamed for Upload.png
 
Top