Partitioning a Schematic in EAGLE/PSpice

[DigiTan]

I'm doing a couple large circuit designs that are too big to put in one schematic. I need some way to break both projects into 5 parts. I'm not even sure if "partitioning" is the appropriate term for it. All I know is it involves naming all the interconnecting nodes and linking the diagrams together somehow. I'm trying to do this in Cadsoft EAGLE and Cadence PSpice. There's a lot of great tutorials out, but I haven't seen one for partitioning.

 

[Boncuk]

Partioning schematics

Hi DigiTan,

making multiple pages of one project using Eagle is very easy. Just left of the library symbol there is the page displayed, normally showing 1/1 if you just have one page.

To create one more page just click the "down arrow" in that window. You'll automatically get the next page and the display indicates 2/2. (Page two of two) This page is completely blank. So the first thing you certainly want to do is adding a frame. Do that like you did with page 1.

If your schematic is already too big and confusing just "group" the part you want to move to page 2. Cut it and save the schematic after having erased the grouped part. (After copying that part to the paste buffer this is still a group and can be erased using the right mouse button.) Reopen the schematic and change to page 2. Then paste the content of the paste buffer onto that page. Erase unneccary nets and replace by the ones you want to draw.

There will be no duplicate parts in the schematic. Just keep on drawing the schematic as if you were working just on one page. You can use this technique also if there are identical circuit parts to be drawn. Group - cut - paste. The new part will have new part numbers and the values are being displayed like the original ones.

If you create a board typing "board;" all parts used on all pages will be within the board.

This is just a hint in case you want to create multiple boards from one schematic. I normally finish the part which has to be placed on the first board and add additional parts for the next one later - after the first board has been created. If you put all those parts into one dimension frame all the following parts will be displayed outside it and ready to make a second board.
That way you don't have to sort out the parts for the different boards.

When the two boards are finished you'll still have some air wires between them. I assume that you will have taken care of that by adding appropriate connectors to the boards. You'll have the air wires despite that. Just disable layer 19 (unrouted) and as a result you'll have two neat looking boards, of course after you have checked a highlighted pad on each board which gives you additional control about what you have done.

I added one example in the attachment. Pic1 shows the air wire connecting SP6 on the L/H board to SP1 on the R/H board. Pic2 shows the same boards clean and neat without air wires.

The content of Pic2 is on page 2 in the schematic.

Kind regards

Hans

 

[monkeybiter]

not my query but thanks for that imediately useful answer.

 

[justDIY]

yes, thanks for the great tips Boncuk!

 

[DigiTan]

Okay. I think that answers the Eagle question. The only thing is, when I click the 1/1 in the drop-down list, nothing happens. Is there some other way to trigger a new sheet?

 

[justDIY]

quoting from the CadSoft website:

The EAGLE Light Edition can be used for free!

Limitations

The following limitations apply to the EAGLE Light Edition in general:

* The useable board area is limited to 100 x 80 mm (4 x 3.2 inches).
* Only two signal layers can be used (Top and Bottom).
* The schematic editor can only create one sheet.

 

[DigiTan]

* Awkward Pause *

New topic: Who's willing to send me $600? Anyone? Anyone?


Well, I guess the EAGLE multi-sheet will have to wait. Anyone know how to do it Cadence's PSpice?

 

[jpanhalt]

Click on "non-profit." It's $125 and offers most conveniences. Of course, you have to use it for personal, not commercial use. John

 

[justDIY]

Another suggestion for you ... the schematic "area" can be of unlimited size. Why not break your complex schematic down into partitions like you're thinking, and just space them out a little on the sheet. draw a frame around each partition using the wire command. you'll now just have to zoom in / zoom out of the different sections.

 

[jpanhalt]

Why not break your complex schematic down into partitions like you're thinking, and just space them out a little on the sheet.

I have done that too, but when it comes to printing, I have not found a way to print only part of the whole schematic. It gets too small to read. The only solution I have found to that is to cut, paste, print. That's a minor inconvenience, but inconvenient nevertheless. Do you know another way to print only part of the schematic? John

 

[justDIY]

I have done that too, but when it comes to printing, I have not found a way to print only part of the whole schematic. It gets too small to read. The only solution I have found to that is to cut, paste, print. That's a minor inconvenience, but inconvenient nevertheless. Do you know another way to print only part of the schematic? John

I've learned to put up with a certain level of inconvenience to save some cash

 

[DigiTan]

Yeah, I guess I could do that. If nothing else, I could printscreen it to MS Paint and just label the nodes and busses with text.

 

[mneary]

I also use huge schematic inputs, partitioned. I made a multi-page template with all the frames in the right place, and put it in frames.lib. Not all printers have the same printing area so it may require some adjustment.

To print, deselect auto scale. Make sure your printer driver is set to 'print preview'. When the print preview comes up, delete the pages you don't want.

 

[Boncuk]

Okay. I think that answers the Eagle question. The only thing is, when I click the 1/1 in the drop-down list, nothing happens. Is there some other way to trigger a new sheet?

You are almost on the right way. Just click the down arrow next to the 1/1 window. You'll get a small drop down menu with the page you already have "1/1" and the word "new". Select "new" and you get an additional page.

 

[bobpen007]

bobpen007

to work with multiple sheets you can move a part of the current sheet to any other by:

1. push move button
2. under move Function push the select button
3. right click mouse to do group move and start dragging the selected area
4. move the mouse to the sheet selector button and select the page you want to move
5. after selection you will see the new sheet and the move group will be active on it
6. drop the group on the desired place on the new sheet.

The elements are moved to the new sheet and did not longer stay on the old one.
The names of the elements are the same - no increasing on the name number which mean the same element was moved from one sheet to other.