London Power ad

[-]
Search the Forum








(Advanced Search)

Schematic management
#1
Hi Guys

Part-1

When we draw a schematic by hand we are limited by the paper size as to how much circuitry we can comfortably fit onto the page. Symbols and text have to be large enough to read clearly, preferably without the need for a magnifying glass. Hand rendering usually invokes our sense of proportion and we try to keep similar symbols the same size as each other, and try to have room for what needs to be shown. We try to organise the circuit flow so it easy to follow and often use connection symbols such as GND and V+ to show things that are tied to each other without having to pull a line all the way across the page.

With computer software, and PCB design programs like Eagle, schematic entry is much the same as hand rendering except that we go to a library within the program to find symbols, then 'drop' them in place. Then we connect them with 'nets'. As we add more components we run out of space as far as the scale of our view goes, because Eagle defaults to a certain effective page size. We can zoom out and add more parts then use the 'fit' function to resize the circuit to the screen size. Things are smaller now, but likely with modern monitor sizes we can still read component names and values. However, it is very easy to get to a point where you have to begin zooming in to read text, and that becomes a problem if you ever want to print out the schematic.

In drafting, there are standard size "sheets", or paper sizes. 'A' is the same size as a North American letter size, 8.5" x 11". The orientation can be long-side vertical (portrait) or long-side horizontal (landscape). Size 'B' is twice the area; 'C' is four times; 'D' is eight times and 'E' is sixteen times. Obviously, for hobbyists and home users, printing anything other than 'A' size is impossible  Yes, there is 'legal' size paper and in Europe size A4 is slightly larger than letter size.

Eagle provides a facility to have multiple sheets for the schematic. This allows you to break the circuit into smaller portions that can be printed more easily and more legibly. When we need to make a connection tie from one sheet to another, we use "ports" or "wire links". These are DEVICES in the Eagle library that let you have these page breaks yet on the board the same-labelled ports are tied together by a trace.
Reply
#2
Part-2:

Eagle provides a means for you to keep the schematic on a reasonable size scale per sheet through direct or indirect means.

In the library is a folder called FRAMES. These are the outlines and information blocks you see on drawings from companies with lots to keep track of Smile There are several different styles of frame to choose from, so when you begin the schematic entry, you first go to FRAMES and drop one in place. Then you enter the schematic within the frame and once it is as full as you need or can stand, open a new sheet, drop a frame and continue entering the circuit.

An alternate method to keep the sheet within a printable size is to draw your own frame on the NAMES layer, which makes the frame a grey line that won't be confused with nets.As you draw the line you will see the cursor x.y position in the top left corner of the window. You can make this simpler and quicker by setting the scale much larger than usual, say 1" and keep the bend function at the default of perpendicular. Draw the rectangle for the size of sheet of paper you want to print on, then switch the scale back to 0.1" to drop components and lay nets as usual.

REMEMBER that the scale for schematic entry must be 0.1" or Eagle won't be able to tie to the component pins.

Oddly, the PORTS are found in the FRAME folder as well. There are a few of these but you can also make your own connection devices. In my parts file, I have "wire links" that are a DEVICE comprised only of a SYMBOL, but you have to have it in the library as a DEVICE or Eagle cannot access it to drop onto the schematic. So, you go into the library, select SYMBOL and enter the name of the wire-link or portal, Eagle asks if you want to create new symbol named as you've entered, click yes, then draw what will appear on the schematic. A friend of mine simply draws a short piece of net on the NET layer, and adds the PIN at one end. I draw a 'T" and fix the pin to one end. Use the NAME function to name the pin "wire-A", for example. Then use the TEXT box to enter a letter "A" to drop on the NAME layer. You can change the scale to position this more nicely - just make sure the pin is on the 0.1" grid. You can make as many of these as you anticipate needing, or give them functional names as you see fit.
Reply
#3
Part-3

In the case of a simple circuit you likely won't bother with frames or the need for ports or wire links. However, it is very easy to have a circuit becomes wildly larger than a piece of letter size paper. The test is simply to print it out and see if it is legible. If it is not, you can easily break up the schematic and place parts of it on new sheets - as many as required.

To break the schematic apart, you can GROUP and MOVE a portion sideways so it is easier to cut off and delete. before you cut nets between the two circuit sections, add the wire-links. On a given net, add two of the same wire-link to that trace then remove the net in between them. repeat this for any other connections that should stay intact between the two circuit blocks.

Once the two blocks are no longer visually connected, you can GROUP, CUT and GO on the block to be moved. The circuit portion is now in the clip board and you can delete the block from the schematic. Now open a new sheet, then select the PASTE function and the circuit should be attached to the cursor. Left click to stick it in place. Now the circuit is spread over two sheetsbut connections between them remain intact.

If we only have a schematic, we can do things in a slightly different way, but it is better to use the method described if you have already laid out the board, or have begun doing so.

If you are revising the schematic for a completed board, only to make the schematic more readable when printed, then there are a few extra steps that must be made. We will look at that in Part-4.
Reply
#4
Part-4:

Splitting the Eagle schematic into more sheets when there is a finished board layout requires a few extra steps compared to having the schematic alone. Eagle maintains annotation between the board and schematic so that when both are open, a change made to either will reflect in the other. If you make changes to one while the other is closed, then opening both will invoke a warning that the board and schematic are inconsistent and no forward/backward annotation will take place until the errors are corrected.

We open the schematic and the board will automatically open, too. On the schematic, we move around the portion we wish to isolate and move, add the wire-links and make the net cut between them. As a check, we go to the bard and click on the ROUTE function then left click the mouse to see if there is anything disconnected. If everything has been done right there will be nothing to connect and the board and schematic are consistent.

Now we close the bard.

We GROUP the circuit portion to move, select CUT, then GO, and open the new sheet of the schematic , then PASTE to bring in the circuitry and drop it in place. And SAVE.

Re-open the board and see that everything is still consistent.
Reply
#5
Part-5:

In the re-organisation of the schematic and distribution of it over new sheets, we can encounter a problem if there are multi-element devices whose elements are not all on the same sheet. An example of this is a relay.

A relay can be designed as an all-in-one symbol and thus be a DEVICE that has only one element. This is how the original Eagle library relays are formatted. However, the relay can also be composed of two or more elements: the coil, and as many switches as there are poles. A DPDT relay would have three elements then: the coil, the first switch pole, and the second switch pole. The witch poles are the same SYMBOL as for an identical stand-alone switch, so the symbol itself can be used by several DEVICES. Similarly, the SYMBOL for the coil can be used for other DEVICES, such as inductors. How the coils and switches are named within each device makes it clear on the schematic that they are part of something else.

In our schematic splitting, maybe we have relay contacts on the part we wish to move and the coil for that relay is staying where it is. For this scenario, when we get to the point where the circuit to be moved has been isolated, we close the board, then delete the relay contacts from the isolated circuit. Now we GROUP, CUT, GO, open the new sheet and PASTE the circuit in place. Now we INVOKE the relay contacts by pressing the INVOKE function, and type in the relay name and ENTER. A window opens with the relay elements listed, but with only the contacts highlighted as being available to select. We click on the the first contact and drop it in place, then on the second and place it. The circuit is complete again. Press SAVE.

If we do not do the above step, the circuit PASTE will rename the moved relay contacts to reflect a new relay being added to the circuit and the board and schematic ill not be consistent. if this happens, simply delete the renamed relay contacts and do the INVOKE steps above to reclaim the original relay contacts.

Now we open the board again and the board and schematic should still be consistent.

All of this is just a sequence of steps where for a portion the board must be open or closed for consistency to be maintained. Eagle has no provision for a quick solution, but life is an imrpovisation.
Reply


Forum Jump:

[-]
Come in where it's warm!
A warm welcome to those interested in tube and hi-fi audio! Fans of Kevin O'Connor's The Ultimate Tone (TUT) book series form a part of our population. Kevin O'Connor is the creator of the popular Power Scaling methodology for amplifiers.
Please remember these three principles: respect, sharing, community.
Not familiar with The Ultimate Tone book series? See discussion topics, or click here to visit London Power/Power Press Publishing.

[-]
Forum Hosted by London Power
London Power logo