Altium Project Parameters and Import into KiCad

Schematic
1

I recently upgraded to version 8.0.0 and tried to import an Altium Schematic . I wanted to start simple so I tried a Title page I have been using on Altium/Solidworks PCB ( a scrubbed down version of Circuit Studio). In Altium you are able to set Project parameters that can then be used on sheets and in the PCB that are like Global variables. I realised that after import some of my parameters from Altium are recognised while others are not. Where is KiCAD storing these parameters and where can I then go to define them. I have posted a few snap shots of some that worked and others that did not.
For example sheet numbers seem to work fine

image
image1190Ă—615 101 KB

But Project Name and some other parameters are not recongnised
Project_Version
Project_Version987Ă—720 107 KB

2

Is this of help?

ksnip_20240311-144524
ksnip_20240311-1445241126Ă—731 106 KB

3

HI JMK thanks for the pointer. That is what I am using to create a new custom Template. As you can see in snap shot below.

image
image955Ă—267 15.9 KB

I need to know how KiCAD translates the Altium parameters into KiCAD as some like Current date Sheet numbers etc are being converted however some others are not

4

a

b

Oder wenn du das meinst:
void SCH_IO_ALTIUM::ParseLabel( const std::map<wxString, wxString>& aProperties, std::vector<LIB_SYMBOL*>& aSymbol, std::vector<int>& aFontSizes )
in ./eeschema/sch_io/altium/sch_io_altium.cpp @ 1454 - 1554

        static const std::map<wxString, wxString> variableMap = {
            { "APPLICATION_BUILDNUMBER", "KICAD_VERSION" },
            { "SHEETNUMBER",  "#"            },
            { "SHEETTOTAL",   "##"           },
            { "TITLE",        "TITLE"        }, // 1:1 maps are sort of useless, but it makes it
            { "REVISION",     "REVISION"     }, // easier to see that the list is complete
            { "DATE",         "ISSUE_DATE"   },
            { "CURRENTDATE",  "CURRENT_DATE" },
            { "COMPANYNAME",  "COMPANY"      },
            { "DOCUMENTNAME", "FILENAME"     },
            { "DOCUMENTFULLPATHANDNAME",
                              "FILEPATH"     },
            { "PROJECTNAME",  "PROJECTNAME"  },
        };
5

Sorry, I cannot help with that. I think @dsa-t may be able to help.
Mentioning using the @ will alert that member next time they open this forum.

6

@johannespfister . Danke. Unfortunately I lost the little german I learnt a long time ago. However I do see why only certain parameters are converted during the Schematic import while other more custom like parameters are not recognized during the import

7

So I found out that For the “custom” Parameters that are not recognized by KiCad during import of Altium Schematics you can set Text Variables File → Schematic Setup as shown in snap shot below. This is the best fix I found so far for redefining Altium Parameters in KiCad

image
image955Ă—616 16.4 KB

2 Likes
9

@johannespfister . Thanks . That is what I was trying to find. I did further search after your post showing the code sections on the parameter conversions. thanks

10

@jmk Thanks for looking into this. @johannespfister code sections gave me the info I was looking for and based of that I was able to find the Text Variables explanation in the KiCad Docs Advanced Topics section

12

I don’t understand this, “Sag doch” sounds to me like an Indian curry and the last bit suggests that you are at “war” with “Jmk” ? I realy think it would be better for everybody if we all stuck to English.
:mouse:

1 Like