Good morning,
I tested importing schematics and PCBs from Altium and it doesn’t seem to work for me.
I am interested because I have files to import into Kicad because I abandoned Altium.
The import files must come from what version of Altium?
Kicad under W10 64 bits
THANKS
Fraçois
I do not have much experience with altium imports myself. I imported a few of the Nucleo boards from ST once and a few projects found either on the EEVblog or github and it always worked for me. I did a total of maybe 5 imports, but I never did much with any of those projects after the imports. It was mostly a test to see if importing worked. There are limits though. Best I know KiCad does not support all of altiums features, and for some features the import may work badly or not at all.
What is the nature of your problems? Maybe it’s not related to the files or the importer, but to the way you do the imports. If you upload one of the projects you have problems with, then there are several people here who are willing to do the import and have a look at problems. If you don’t want to share your own problems, you can use a random project (for example from github) as a reference so there is some common ground.
Good morning,
I put the schematic file of a power supply with which I am trying to import into kicad.
The diagram is very classic and can be public.
Have a good day
Alimentation.SchDoc (18.9 KB)
This schematic file does indeed not open for me.
I tried this by first starting Eeechema in “standalone” mode (That is without an active project). and then File / Import / Import Non-KiCad Schematic. These importers are not available when KiCad has an active project.
But as I wrote, it does not work for me either.
A short analysis:
paul@cezanne:~/downloads$ strings Alimentation.SchDoc
DProtel for Windows - Schematic Capture Binary File Version 1.2 - 2.05
Times New Roman
CAPACITOR
R-04
R-04
CAPACITOR-POL
HEADER 3
DIODE
and then comparison with a project that does work:
paul@cezanne:~/projects/arm/00aa_projects/00aa_motor/Dummy-Robot/1.Hardware/Controller$ strings Main.SchDoc |head -n10
|HEADER=Protel for Windows - Schematic Capture Binary File Version 5.0|Weight=1994|MinorVersion=2|UniqueID=QVBBULDQ
|RECORD=31|FontIdCount=11|Size1=10|FontName1=Times New Roman|Size2=10|Rotation2=90|FontName2=Times New Roman|Size3=10|Underline3=T|FontName3=Times New Roman|Size4=10|FontName4=Consolas|Size5=10|Rotation5=270|FontName5=Times New Roman|Size6=5|FontName6=Arial|Size7=8|FontName7=Courier New|Size8=5|FontName8=Courier New|Size9=14|Underline9=T|FontName9=Arial|Size10=10|Rotation10=180|FontName10=Times New Roman|Size11=36|FontName11=Times New Roman|UseMBCS=T|IsBOC=T|HotSpotGridOn=T|HotSpotGridSize=5|SheetStyle=1|SystemFont=1|BorderOn=T|SheetNumberSpaceSize=12|AreaColor=16317695|SnapGridOn=T|SnapGridSize=5|VisibleGridOn=T|VisibleGridSize=10|CustomX=1500|CustomY=950|CustomXZones=6|CustomYZones=4|CustomMarginWidth=20|Display_Unit=0
|RECORD=41|OwnerPartId=-1|Color=8388608|FontID=1|IsHidden=T|Text=*|Name=CurrentTime|ReadOnlyState=1|UniqueID=DJIXRFRS
|RECORD=41|IndexInSheet=1|OwnerPartId=-1|Color=8388608|FontID=1|IsHidden=T|Text=*|Name=CurrentDate|ReadOnlyState=1|UniqueID=DPHOGMVK
|RECORD=41|IndexInSheet=2|OwnerPartId=-1|Color=8388608|FontID=1|IsHidden=T|Text=*|Name=Time|ReadOnlyState=1|UniqueID=BGTJBPVO
|RECORD=41|IndexInSheet=3|OwnerPartId=-1|Color=8388608|FontID=1|IsHidden=T|Text=*|Name=Date|ReadOnlyState=1|UniqueID=QKEORCCO
|RECORD=41|IndexInSheet=4|OwnerPartId=-1|Color=8388608|FontID=1|IsHidden=T|Text=*|Name=DocumentFullPathAndName|ReadOnlyState=1|UniqueID=LEDWDDWJ
|RECORD=41|IndexInSheet=5|OwnerPartId=-1|Color=8388608|FontID=1|IsHidden=T|Text=*|Name=DocumentName|ReadOnlyState=1|UniqueID=APGDBRII
|RECORD=41|IndexInSheet=6|OwnerPartId=-1|Color=8388608|FontID=1|IsHidden=T|Text=*|Name=ModifiedDate|ReadOnlyState=1|UniqueID=EPKYLIPM
|RECORD=41|IndexInSheet=7|OwnerPartId=-1|Color=8388608|FontID=1|IsHidden=T|Text=*|Name=ApprovedBy|ReadOnlyState=1|UniqueID=RYQUAKNH
This comparison shows a relation. Both have the “Protel for Windows” string and the “Schematic Capture Binary file Version”. Your “Alimentation.SchDoc” claims to be a: “File Version 1.2 - 2.05”, while the file that does work for me has a: “File Version 5.0”. Therefore I suspect that the file you uploaded is from a very old Protel / Altium version. Is this correct? A simple thing you can try is to open the file in a recent altium version and then save or export it, and try again with KiCad.
The file I compared it with is (very likely) from this project: https://github.com/peng-zhihui/Dummy-Robot
Hi,
Yes, you have right, it’s an import in altium from Protel 99 SP6.
François
I’d suggest using the Protel99SE importer in a current Altium version. if you need it imported, send it to me…
@glenenglish @paulvdh So in your experience what is the best work flow to get an Altium project into KiCad 8 or newer where the Schematic syncs with PCB layout.
So far I have been able to import and create the libraries with just a few edits once imported. What I am tryiing to figure out is how to get the Schematic and PCB into KiCad and have them sync up. I followed documentation advice and first imported the PCB into a standalone then saved the file this created a project file however it also creates an Altium Library file which I am unable to edit . Is there a way to get the PCB to point to the prior imported footprint library?
The second challenge is once I import the flat schematic sheet into standalone schematic editor and save, this creates a separate project file in the same folder as the one created when PCB was imported . How do I get the imported schematic copied into the PCB created project and also link it to the prior imported Schematic library. Is this even possible. ? Is it worth going through all this trouble or should I just import libraries and then recreate the schematic and PCB’s again?
Try it this way:
- Create a new KiCad project, with both a schematic and a PCB file.
- Then import the schematic and the PCB into that new project (Standalone mode not needed).
- To synchronize the schematic with the PCB, use: Schematic Editor / Tools / Update PCB from Schematic [F8] and then make sure the checkbox for the option Re-link footprints to schematic symbols based on their reference designators is on. (And make sure it is off when you do more updates later).
I’d say forget about libraries at the moment. If you wish, you can create libraries later with … Editor / File / Export / Symbols (or footprints) to (new) Library. Links to external libraries are not really needed in KiCad (starting from KiCad V6). Newer KiCad versions complain about missing or broken library links (or when symbols or footprints differ from those in the libraries), but that is a check (I guess) most useful for people who use database driven libraries. It is a perfectly valid workflow to either ignore or disable the checks for this.
If you run into further specific problems, then it’s probably better to create a new thread for it, instead of tagging along on someone else’s old thread.
@paulvdh Thanks so much for the pointers. I will try that. Good point about a new thread if i still run into issues. Well noted