[SOLVED] Schematic symbol will not load onto PCB

[Capsized]

In the process of working on an energy harvesting system, I created a symbol for the LTC3901 component (DIP20 footprint). Working on the schematic is fine and the rule checker runs without error.
Then, when importing into the PCB editor, it runs without error again. However, the LTC3901 does not correctly import as it does not show up in the PCB editor. When I go back to the schematic kicad automatically has updated its name from ‘H1’ to ‘#H01’.
Looking into it, there is:

• No other symbol name conflict
• I have correctly assigned a footprint in both the symbol editor and the schematic
• I have no special characters on the symbol

Please let me know what I should do to fix this !
Thanks

[paulvdh]

The title of your thread is strange. “Schematic Symbols” are never loaded into the PCB Editor. The PCB editor only loads the footprints attached to schematic symbols. Because of this I am confused what is actually happening.

And what bout the DIP20 (which is a footprint). A short check suggest the LTC3901 is delivered in an SSOP-16 package.

[mf_ibfeew]

only guessed: is the “power symbol” checkbox set for your self designed symbol?

To guide you to better answers I copy something I wrote yesterday:
You will get the best help if you attach your project (Kicad main manager–>File–>archive project) in your post. So we can look into that schematic/symbol and look for the cause of the problem.
As a new user you have to get the next user-level first (as anti-spam countermeasure). Read and followthis link: New Member Information.
If you have promoted yourself to basic user level you could attach your project.

[Capsized]

Thanks so much for the link, I have now attached the archived project to the post .
Also I have checked and the power check box is ticked for the component

[Capsized]

Haha sorry my mistake, it is the LTC3109, regardless, I’m still new to KICAD and so I think some of my terminology is wrong.

[paulvdh]

If you look at the properties of your #H01 symbol, then you see that both the Exclude from BOM and Exclude from board checkboxes are set.

But changing those does not help much. I can confirm that mf_ibfeew is right and this symbol is defined as a power symbol. To fix this:

1. Hover over it and press [Ctrl + e] to load it in the schematic symbol editor.
2. Symbols Editor / File / Symbol Properties

3. Close the symbol Editor. (KiCad asks you to save the changes into the schematic, answer with [Yes].
4. You also have to change the #H01 to remove at least the hash sign. After these changes the DIP20 loads into the PCB editor. To do it properly, you should also export the schematic symbol to a library and give it it’s proper LTC3109 name.