I was in the middle of soldering a PCB I designed when I realized I forgot to decouple the RFM69HCW module with 0.1uF. Does anyone have any insight to how damaging this is, and if I need to redesign and redo my board? I'd prefer to not have to spend the time and money if I don't have to. The 3.3V is being supplied from the external circuit of a TPS563200 (step-down converter) on a 0.3mm trace, 15mm in length. The board is grounded by a ground plane, though the connection to the plane is rather far away as it passes through 5 smt components before connecting to a grounded TH component. Is this okay for me to move forward or should I redesign my board?
Try it out to see whether it works or not before doing a redesign. You cannot damage anything just because of a missing decoupling capacitor.
EDIT due to comment: The above sentence assumes, that your power supply is properly designed and stable.
The worst thing that could happen, is that the module could show weird unreproducible behaviour from time to time due to undervoltage resets.
However, I think your design will work either way since the module you're talking about has decoupling caps on board.
Edit after posting schematic and layout:
By reading the comments of your original post, I can see that you will do a redesign anyway due to a badly selected level shifter.
I see a couple of improvements that you can do on your layout:
1.) Grouping: Try to give your layout more structure by grouping together what belongs together. Make physical sections to separate the power supplies, the microcontroller stuff and the RF transciever. You can then route each section individually and your board will probably look tidier. Try to separate the DC-Converers, the Clock and the RF transciever.
2.) Decoupling capacitors and grounding: Connect all your capacitors directly to the ground plane on the bottom layer through a via. Each capacitor (and each ground Pin of each IC) should have it's own ground via. Try to make the bottom layer a ground-only plane and avoid routing of other signals there. See this article for the image source and more information.
3.) Power supply: All DC converter IC's have strict layout guidelines that should be followed in order to lower the switching noise on the output. A recommended PCB layout is typically shown in the datasheet. Stick to it. Additionally, I can suggest you to read this article about DC/DC converter noise filtering. It is also important to use the correct parts (Inductor + Capacitor) for output filtering. Also here, the datasheet typically provides formulas for calculating their sizes and sometimes also part numbers. If you are unsure, you can also use freely available (but often vendor specific) simulation tools such as the WEBENCH power designer from TI. The simulator will give you information about the expected output noise and will also suggest the filtering component sizes and part numbers.
It seems to be necessary to do a new board anyway if you want to fix any errors.
Otherwise you could just solder on extra bypass caps and hack the board to work.
For example the regulator feedback pins are incorrectly connected, the MCU can't communicate SPI via level shifter, the level shifter has unused pins left disconnected, and the 3V3 data pin is not shifted up to 5V level for the MCU. Usually 5V MCUs cannot work with 3.3V input levels. This is not an exhaustive list and there may still be serious or less serious errors.