Continue to Site

Welcome to our site!

Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

  • Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

Eagle, circuit isolation.

Status
Not open for further replies.

HerbertMunch

New Member
Hi i have included the schematic of a pic USB device, that i found on the internet.

Can someone tell me how the author has managed to isolate the different components of his circuit, i.e wires do not directly connect pic>d+ to usb>d+.


Many thanks
 

Attachments

  • PicWinUSB_Sch.jpg
    PicWinUSB_Sch.jpg
    51.3 KB · Views: 391
look at net name.. if they are the same, then they are electrically connected no matter what the schematic looks like.
 
If I understood the question.

On the schematic:
All wires with the same name are connectect together, but the wires between them are not shown.

the D+ wires on the USB connector and the PIC both have the same name. When you layout the board the airewires/rubber_bands will be there to ensure you make the connection.

The tag things with signal names generaly indicate that this is the case.

This makes for a much easier to read schematic.
 
Perhaps it is called detached drawing of a schematic.
this technique was followed in telecom since log time
 
I've been using that style more and more recently, it makes for a much cleaner and compact schematic... clear and concise labels are a lot easier to follow then trying to follow signal wires (all of which are the same color) around on a diagram.

another useful eagle feature is the BUS command, you can define a bus to carry multiple signals, represented by a single fat line ... connecting two or from this bus brings up a menu prompting what signal you want to connect to.

the only thing I'd like to see is the ability to color code the bus 'wires', if you have to buses on the same schematic, it would be nice to have them different colors, in addition to having them labeled.
 
I find using the eagle command line to be the easiest way

1) place your parts where you want them
2) type net 'mynetname' - you can just type this on the eagle screen, doesn't matter what tool you're using or anything, eagle will switch to the net tool automagically
3) start a few ticks off the pin your want to connect to and click, now draw your signal line to the pin, clicking again when you get there.
4) now press the up arrow, or type the net 'mynetname' command again, eagle will switch to the net tool
5) repeat step 3 for the second part
6) now go into the eagle libraries and find the labels or callout library (cant remember off hand), and put 'em in the schematic, or just use eagle's label tool

alternately, you can do it all through the gui

1) click on the net tool and draw a signal line on your first object - double click to terminate the signal line without connecting it to anything
2) click on the name tool and then click on the signal you just drew, give it some same
3) now draw another signal line using the net tool for your second object
4) repeat step 2 for the line just drawn - eagle will prompt you, something like "connect signal n$1 to mynetname?" ... answer it yes and you're done.

this is easier to visualize if you can fit both the schematic editor and the board editor on the screen at the same time - then you can see eagle place air wires between parts as you define the signals on the schematic
 
Status
Not open for further replies.

Latest threads

New Articles From Microcontroller Tips

Back
Top