I’m trying to create atomic libraries of resistor and capacitor symbols that don’t require any editing after placement on the schematic. The symbols are to be populated with house part numbers, footprints, etc.
For instance: My symbol name is R805-47k-5%. I’d like to have the Value=47k. I can create a symbol like this in V6.0.4 but the Value is overwritten with the Symbol name when the component is placed. The Values are used for SPICE simulation so having the Value overwritten breaks simulation unless I manually edit the symbol. Having to edit the Value manually partially defeats the value in having atomic libraries.
I’ve seen discussion of this issue related to version 5. It was claimed that version 6 would support having different Symbol names and Values. It appears not to be an issue with the new library format, but the place symbol behavior is still preventing my desired behavior.
@circlotron I’ve got the exact same issue! Haven’t found a way around it and therefor I’m still using LTSpice for simulation and not KiCad.
I once tried editing a library in a text editor to set the value differently than the name. It didn’t work. When I added the symbol to the schematic the name and value was still the same. I don’t remember which of the values that Eeschema used though.
I would like the name to be our House Part Number and the value to be the actual value (on components that has a value). On top of that, I want the name to be shown in the schematic, and not the value. I’m not sure, but as of today I believe only the value van be shown in the schematic.
@iabarry Ref designators has nothing to do with it. What we want is the ability to set a different value (i.e. 100k) than the name of the symbol. In the symbol libraries the name and value is currently always set to the same string.
As others already said: not possible in v6. Seems it’s hard coded that Value == Symbol in the library. workaround is to use an own property “MyValue” and set this property to visible.
How this would work for simulation - I don’t know as I don’t do simulation.
What will you do for 47k in Smd and Tht? How will the BOM work? This is just a bad idea.
Because you see problems it’s not immediately a bad idea. Always bear in mind: different people - diferent workflows.
I would also like the possibility to define Value != symbolname in the library. Building the BOM (and distingusihing SMD from THT-parts) is done with additionally library-properties: we have defined an MF==Manufacturer property and an MPN==Manufacturer Production Number for every library part.
Main advantage of Value!=symbolname for me: much less cluttered schematics directly after inserting symbol from library. No reworking of value necessary (only valid for fully defined atomic parts, not for generic symbols). Look at the example-picture. The long value on the left capacitor disturbs the picture and is redundant information (as the MF+MPN property is still present in the background, ready for bom-creation).
If I understand it correctly, this does not work with simulation. I believe the value used in the simulation is always the “Value” attribute. But if we could somehow change which attribute the simulator gets the value from, that would probably be a solution.
The only solution I know of currently is to add the House Part Number as a custom attribute, and set the name+value to the actual value. That solves it for me, but has the hughe drawback that its a real pain adding new symbols to the schematic since they are then listed by their Value and not the HPN.
I can see the benefits of a database driven parts management system, but KiCad is not there yet.
I have no experience with it, but I think that using a separate field for house parts numbers would then be better. I really like the simplicity of just entering a text string for resistor and capacitor values, and being forced to use house part numbers for initial drafts and simulation for projects that may never see production disrupts the creativeness of the design process.
If a database system is ever added to Kicad, then parts can be dressed up later and the value field can for example be used to make a pre-selection from the database parts.
Adding some scripts to flag discrepancies between the value field and the HPN should then also be added.
Thanks albin, I saw the older discussion (now closed). I also found a similar thread that indicated the library format was the limiting factor and that this issue would be addressed in V6.0. I’ve looked at the new library format and it does seem to be addressed there. Just trying to see if anything had changed yet.
Every other ECAD software package I’ve used has made a distinction between the name of the symbol and the SPICE Value. This seems like an odd quirk. I don’t understand why this should be mandatory as you can manually fix each part in the schematic after placement.
What is the procedure for submitting an enhancement request?
Just to clarify - I’m using the reference designator in the normal way.
You can change the value that spice gets for simulation. If the symbol has certain Spice_* fields, spice will use for model information rather than guessing what builtin model to use based on the refdes. Specifically, the Spice_Primitive field is used to define which kind of component it is (here R), Spice_Model is used for model parameters (here 1 for a 1 Ohm resistor), and Spice_Netlist_Enabled for whether it should be included in the spice netlist.
You can add these fields yourself or they get added for you by the spice model editor dialog.
This simulates fine even with a nonsensical Value for the resistor:
That is awesome! I believe that solves it all for me! I’ll make sure to include thous three attributes in all our atomic libraries. Now I just need to learn how to use KiCads spice simulator.
Sure, my point was about “Value” and “Datasheet” fields being mandatory.
I don’t use them in my workflow but people need to be free to add them if they use them.
I’ll make sure to include thous three attributes in all our atomic libraries. Now I just need to learn how to use KiCads spice simulator. 