Please try with 74HC74_3part and edit attributes to suit your choice of part

How can I use the SN74HC74D with subparts without having a new IC in PCB for each subpart?

There are a number of problems with your SN74HC74D schematic symbols. The SN74HC74D part that is in your name (i.e. the one that was in your personal library shown in your original post above), is assigned the D014_N SMD package. In the screenshot of your PCB example, it no longer calls up the D014_N SMD package but is calling up a through hole package. Close inspection shows that the pins are slightly off grid in the vertical axis.    * Please correct this grid misalignment. Close inspection of the EasyEDA Source file for each sub part symbol shows that they have all been assigned the same sub part prefix "pre" and number "subpart_no":    * If you edit these attributes so that they are in the same form as for the 74HC74_3part symbol then only one package should appear in the PCB:    Like this:  

How do I open the "EasyEDA Source file for each sub part symbol" ? Thank you,

please make sure the subpart's pre is correct, when you place it on the schematic, they must be U1.1, U1.2, U1.3, [https://docs.easyeda.com/en/Schematic/SchLib-Search-And-Place/index.html#Multi-part-Components](https://docs.easyeda.com/en/Schematic/SchLib-Search-And-Place/index.html#Multi-part-Components) if when place the subpart on the schematic, the prefix change to U1.1B, U1.1C, you need to check the subpart's pre when edit it.  they must set the pre as: U?.1, U?.2 etc.

@peternarbus,  When you create a symbol with sub parts, please first create an empty symbol with a package assigned to it like this:  At this stage, you can enter the package text directly by left-click-and-drag from the right-hand end of the package name (by default this is NONE) in the Package attribute text box or by editing the EasyEDA Source file. Then search for and select the new, empty part and right click on it to create a new sub part:  Then select the new sub part and edit it in the usual way for a schematic symbol:  Repeat this for as many sub parts as are required.

@UserSupport   Thank you - that worked!!

@UserSupport, Editing the "Pre" attribute in the symbols placed in the schematic allows Peter to use the parts in his schematic but it does not fix the User Contributed symbols in the library so other people picking up this part will have the same problem. @peternarbus, It would be good if you could make the changes identified above to fix the symbols in the library. Thanks.

@andyfierman. Ok, I will try to correct the source for the subparts.  Thank you. Note:  This part was created from an import of Altium ASCII.  I don't know if the problem came from th Altium export or EasyEDA import...