Further testing led me to check the import of schemes from altium … When I try to convert several schemes one after another, the first one is erased … Let’s say a root sheet is created, I import the scheme there, I create a second sheet in this import scheme and my second sheet replaces the first … Is this a bug or am I doing something wrong ? How to intentionally import multiple Altum sheets into one schema?
Maybe try saving each individual imported schematic as a kicad file? Then the individual saved kicad files can be used. I’ve not tried this myself so let us know if this works.
Yes, it happened offline … True, in the folder a bunch of files turned out with libraries of symbols from each scheme … It imports them without asking when converting
When I try to convert several schemes one after another, the first one is erased
Do i understand that correct: You open KiCad, import a Altium schema, you can view it, then you store the schematic as a new .kicad_sch file, then you use the same KiCad instance to import a different Altium schematic and the file you create before gets deleted? Or when you save the before created kicad_sch is overwritten?
Is there a possibility for you to upload some files which you have trouble importing into KiCad?
You have opened a schematic project imported schematic number 1 from altium added a second sheet to kicad and imported schematic number 2 from altium… And then I expect circuit number 2 to appear on the second sheet of kickad but instead circuit number 2 replaces circuit number 1… .
_Base_Board.zip (80.0 KB)
I can’t say for sure whether it is overwritten or deleted, but it becomes inaccessible
Please try to be as specific as possible. In a way that is exactly clear what you do, what happens and what you did expect to happen instead. You are very vague.
Here is what i understand:
- You created a new KiCad Project.
- Then you open the schematic editor eeschema (The schema editor of KiCad).
- Then, inside eeschema, you import a Altium schematic file.
Then i don’t understand which of this things you do:
- You created a new schematic sheet by placing a hierarchical sheet on the current schematic.
- You opened up a new instance of KiCad.
- You didn’t open a new schematic nor eeschema instance and replace the current one.
- Some other attempt i didn’t think of.
In case of 1: Yes, you loose that link after importing. You have to: import->save as , open top sheet, add a link to the new hierarchical sheet.
In case of 2: The 2 instances of KiCad should not touch each other and one should not close the other.
In case of 3: That the instance now holds the data from the second import. And only this schematic.
Keep in mind that importing a schematic means: “Open this file and view/edit it instead of the current one.” Maybe this is what you didn’t expect?
Other small bug
I found a small “bug” or unexpected behaviour on my version (which is out of date): When i create a KiCad project, create a new schematic for it, place a hierarchical sheet on it, open that hierarchical sheet. Then i use the current eeschema instance to import a Altium schematic but when i now save, it overwrites the top sheet of the current project (i would expect to either overwrite the hierarchical sheet or to ask where to save it).
I guess the last mentioned “Other small bug” isn’t the one that explains your problem?
yes, your mistake repeats my behavior… that’s what I wanted to say… version 7.0.7 win 64… now you need to try to formulate a description of the error on gitlab… since I write through a translator, there may be some misunderstanding…
KiCad does not currently support “flat” schematics like Altium does.
If your Altium design is hierarchical, you should be able to import it in one step, by opening the top-level sheet in the KiCad schematic editor.
If your Altium design is flat multi-sheet, unfortunately right now the process is more tedious.
You must open and convert each Altium schematic one by one, and save each one to a new KiCad schematic.
Then you must create a new KiCad project, and copy these schematic sheets into it as subsheets of a KiCad root sheet.
2 Likes
Thanks craftyjon,
This is what I was trying to say in my reply above. Now I’m inspired to try this myself.
I understand correctly that the altium circuit file must be physically one? Even if the schemes are interconnected in the form of separate files, then the cicada does not know about it?
If your Altium schematic is “flat”, meaning it has multiple sheets that are not contained within one “top-level” sheet, you need to import them one by one and then add them as hierarchical sub-sheets to a new KiCad project. KiCad can’t directly import this type of schematic automatically (today).
In this example you need to open each of the 4 sheets individually, save them as kicad_sch files, then create a new KiCad project and place these 4 sheets in to the KiCad top-level schematic, as sub-sheets.
If your Altium schematic is hierarchical and has a single top-level sheet, you can open this single sheet in KiCad and the subsheets should be handled automatically:
In this example you can just open “Temperature Sensor.SchDoc” to create a new KiCad project.
Thanks a lot !! Can this be considered a bug or is it a request for a new feature?
There is an existing feature request to import an Altium project in one step: Import project from Altium (lp:#1755952) (#2117) · Issues · KiCad / KiCad Source Code / kicad · GitLab
one more small question… is it possible to convert altium schema symbols to kicad from a library file? Thank you
It is not possible yet but is being worked on for KiCad V8.
(note that if you import a schematic, you can then export all the symbols in that schematic to a KiCad symbol library)
1 Like
yes, your mistake repeats my behavior…
I have no idea what that means. Which mistake? You are saying i did a mistake, but i don’t see one.
now you need to try to formulate a description of the error on gitlab
Which error? I don’t see anything that behaves in a way that isn’t expected.
since I write through a translator, there may be some misunderstanding…
Yes. I understand that you have trouble translating from/to English. But please, when you try to communicate something, especially bug descriptions, try it to make it as hard to misunderstand as possible. You can do that with things like: Saying the same thing twice with different words, writing a extra sentence with the same meaning but in a different form with different words. Use lists to describe what you did in which order.
I wouldn’t be able to give a clear response in a reply as long as this one, no matter which language i would use.
Can this be considered a bug or is it a request for a new feature?
If you ask me: It is a bug in the design rather than in KiCad.
A design should not be flat. Even when ignoring the software. You always should have a single sheet that includes everything. The details can be hidden in hierarchical sheets, but don’t combine different schematic sheets without a clear, explicit described, way how they are connected. I.E. every project should have a single top-level sheet and all other sheets should be subsheets (and subsubsheets, …) of it.
A multiple sheet schematic that has different sheets that are “randomly”, implicit, connected is bad practice.
Other small bug
I found a small “bug” or unexpected behaviour on my version (which is out of date): When i create a KiCad project, create a new schematic for it, place a hierarchical sheet on it, open that hierarchical sheet. Then i use the current eeschema instance to import a Altium schematic but when i now save, it overwrites the top sheet of the current project (i would expect to either overwrite the hierarchical sheet or to ask where to save it).
I guess the last mentioned “Other small bug” isn’t the one that explains your problem?
I wanted to say about this error or bug in the post above … thanks
You have to use a different eeschema instance, not the one you have the new project open in.
(or, you can use the same instance, but close each schematic before importing the next)
1 Like
IMHO: Importing a non-KiCad project and saving it shouldn’t silently overwrite the previously opened schematic.
Do you think that is the behaviour the user expects? Would it be hard to implement a “This will overwrite <someFileName>. OK|Cancel|Save As …” warning / dialogue box when the user tries to save it ?
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.