Hi,
I want to rearrange my subsheets
Can I reorder these subsheets?
For example
Now, I have MCU is in 5/7
but I want that MCU page is in 2/7 ( 7 means total page , 2 means second page)
1 Like
In true hierarchical design this does not matter at all. (sheets are objects not physical sheets of paper. It therefore does not really matter what page something is on.)
Meaning i assume you want to use hierarchical sheets to design a multi page project. The cleanest implementation of this in kicad is by having the root page as a sort of index page. The position of the sub page instance on that index page determines the page numbers.
The automatic annotation tool is what generates the page numbers meaning if you move your page around on the index page you need to re-annotate the schematic for this change to take effect.
For reference the FAQ article: Hierarchical or flat schematic design, what is best for me? (How to deal with multi page schematics?) (in your case look at the multi page flat design part of the guide.)
I do remember there was a GUI tool for this, but I don’t have a link to it and I did not find it with a quick google search. I do not know for which OS it was, and if it is still compatible with V5 (I do recall that it worked with V4).
You can do it manually if you delete the sheet, save the design and then restore it back. The last created sheet has the highest sheet number.
Not quite the full picture. The last sheet added to the annotation is what gets the highest number. It can be the last page added but on reannotation will reorder the sheets depending on the order the algorithm finds them. Which in turn depends on the order they are placed in their root sheet. (Keep existing annotation means no change to existing page order.)
And by the way if you insert a sheet into an already placed sheet (so if you use hierarchical subsheets inside subsheets) then the new page is not necessarily added to the end even if you have keep annotation selected.
Hi Rene
I’ve changed position of the sub page , but there is no difference with the page numbers…
I’ve changed position from Left picture to right one . but there is no change with the page numbers
Could you tell me more details? or let me know what I misunderstand.
Thanks
I think I should study about GUI tool, I don’t have experience with it
Thanks MitjaN
As mentioned above: The page number is tied to the annotation. To change it you need to re-annotate the schematic.
1 Like
I’m also interested in this.
I have a multi sheet design, with a few pages of “important” stuff, and a few pages with “bits and ends”, and when I print it, I want the important stuff gets printed first.
If annotation is the key, how do you re-annotate sheets, without clearing the rest of the annotation?
When I go to:
Eeschema / File / Page Settings
I see:
But no obvious way to change the sheet numbering.
Sheet numbers are in the title block, and changing these directly in the schematic file with a text editor may be the simplest option here.
Edit:
The simple method below does not work. It changes only the text in the titleblock on the screen, but not when sheets are printed (to pdf). According the the Eeschema manual sheet numbers are also appended to local labels to make them unique for each sheet, and this should be considered when trying to change this.
About 5 minutes later:
If you open a schematic file in a text editor, the header looks like:
So I got daring and changed line 5 of all sheets in the .sch files of my project, saved them, and re-started KiCad, and the sheet numbering was as I made it.
No guarantees, always make backups before you do such things.
Complete file formats are described on the KiCad site, but I did not study them very closely (yet) Maybe KiCad gets confused in a sublte way by changing things like this.
1 Like
My experiments do not reveal a way to separate page numbering completely from part numbering.
1 Like
Hi, paulvdh
I’ve tried your method.
I found that
I can change numbers in note editor , so I checked it changed in schematic
but when I make pdf (make plot button) there is no change in relation with the page number.
I think this way can not change plot sequence.
or do you know where I can change plot sequence in note editor ?
Thanks
Raised as a wishlist bug
Feel free to upvote it.
1 Like
I had a short peek at the file format http://www.kicad.org/help/file-formats/ and I could not find a quick way to hack the sheet numbering directly with a text editor.
Also upvoted David’s whishlist bug.
2 Likes
I think that V5 and below just don’t support controlled page numbering, so a file format change will be needed. This means V6 at the earliest, so recording the wishlist item is the best that most of us can do
1 Like
I have a similar need to re-order sub-sheets. I want to impose a sequence so that the sub-sheets are in the same sequence as appear in the root sheet and also as their connectors appear on the final hardware. In my case, I have two temperature-sensor channels and three pressure-sensor channels, all of them using identical circuits and so all of them based on the file Inputs.sch. It makes sense that they be organized with the temperature channels side-by-side and the pressure sensors side by side in the root sheet and on the equipment. However, I am getting the sequence “T1 P3 P1 T2 P2 P2”. How can I accomplish this?
What are the rules that define the order in which the sub-sheets are numbered?
Best regards,
Peter
1 Like
The numbering order is defined by the order in which the sheets appear in the parent schematic file.
AFAIK, to change it you need to edit the schematic file in a text edit, locate the sections starting $Sheet ending with $EndSheet, and arrange them into the desired order.
Editing the file directly carries some risks, so close the file in KiCad file first, make a back up of your project. Use a text editor like NotePad++ (or equivalent for your OS), and not a word processor like Word.
4 Likes
I don’t think that the position of the sub sheets in the root schematic controls the sequence of the sheet numbers. My evidence for this is that:
- I have experienced sheets being annotated in a sequence that does not reflect the root sheet.
- the sequence seems to change from time to time as I edit the sub sheets, without having done anything to the root sheet.
- When I add a component on a subset, the Annotate tool assigns a 3-digit number that reflects the position of that subsheet in the list of sub sheets under Root. However, the first digit of the number is different from all other components on that sheet. For instance, a recently added capacitor might have the reference C401, whereas all the rest of the capacitors on that sheet have reference C5xx, one of which references is C501. So the sheet must have changed position in the hierarchy since the original components were entered.
How can I prevent this from happening short of entering all references manually and never using the Annotate tool?
Best regards,
Peter
I already told you the answer. If you don’t believe me, I cannot help you.
It’s not the physical position on the displayed sheet. It is the order they appear in the file. I’ve successfully renumbered sheet pages by hand editing the schematic file. I wouldn’t suggest it though, it is a pain in the sits-upon and prone to error. And, I’ve had the program re-shuffle the sheets on subsequent saves requiring repeated hand edits.
Best bet is to upvote the issue on Launchpad. I would, but I already did a while ago…
2 Likes
Unfortunately, that bug has been marked duplicate, and attached to a rather different wishlist item of the “probably will never get implemented” variety.
It might be possible to script it, if there is a way to specify the desired order.
I do not agree that this should be marked as a duplicate. I informed michael about this and gave my reasoning. Lets see what the final verdict will be.