Thank you for a wonderful tool.
A Raspberry Pi Pico has seven interconnected GND pins.
Can I in any way make Freerouting route to the nearest GND pin, not necessarily the one I have connected to in the schematic?
I have tried many different approaches, but always ends up without any connection or that all the GND pins gets connected, the later just being waste of space and tracks.
Is there any way to do it?
Delete 6 of the GND pins? Even if you routed manually, DRC would complain you have not routed 6 pins.
Personally I’d just route all of them. Don’t you have a GND plane which is close to nearly every pin?
It is not wasting space but making design better.
At signal lines you have pulses. Pulses contains lot of higher frequency harmonics. To minimize emitted by PCB disturbances and to minimize sensitivity to interference (from external sources and also from neighbouring lines) it is crucial for each signal line to have as close to it GND connection to allow that line current to get back to the source the lowest possible impedance way.
For example when I place at PCB the microcontroller that has many VCC+GND pin pairs I give each pair a capacitor and connect each GND pin to GND and all VCC pins together.
At the center IC on the following picture you can see 6 such constructions (2 at top, 2 at left, 1 at bottom and 1 at right):
Some PCB fabricators will charge you more if you have less copper on your PCB . . . they don’t add copper to the PCB they remove it, do them a favour and give them less to remove 
No. All you can do is run Freerouting and then re-route the tracks afterwards, yourself, by hand. so why bother with Freerouting?
It is not a waste of space and tracks.
NEVER, EVER rely on the internal Gnd. connections to replace PCB tracks for conducting.
Reason 1: Have you ever looked at a video on youtube showing how fine the wires connecting the silicon to the pins on a chip are? They are totally unsuitable to use to connect one external part of the PCB Gnd. circuit to another.
Reason 2: The pins labeled Gnd. are to be connected to Gnd. There is no reason to believe they are internally connected together. Without knowing exactly how the IC is manufactured, you have no idea if the Gnd. pins are internally connected. They may all be connected to different parts of the silicon and be totally isolated from each other, so possibly the IC will not work unless all the pins labeled Gnd are externally connected to each other.
Of course. Throw Freerouting in the bin and draw the tracks yourself, first making sure all the Gnd pins are connected together with tracks on the PCB.
Edit: I re-read your title. You are using a module on which an/some IC/s is/are mounted, not a single IC. So a different question:
Are all the Gnd pins on the module connected together, and if so, are those PCB tracks on the module suitable, and capable of, carrying the current from one part of your design to other parts of your design?
Unless you can say yes, with absolute certainty, never consider using the module as a Gnd. jumper track.
This question appears in a simpler guise when such tactile switches are used:
Electrically they are SPST switches, but they have 4 pins, in pairs, for mechanical mounting. Thus the footprint has two of pin 1 and pin 2.
People have asked how to use only the nearest pin 1 or pin 2. In normal usage the contacts carry negligible current so it is alright to use only one of a pair. However clever schemes just end up being confusing and the simplest solution is to route both pins of both pairs. Rarely is there insufficient board space for the albeit redundant traces joining up the pairs. Either that or ignore the DRC message about pads not connected.
This is a quite silly limitation in the footprint in KiCad’s library for this switch. This switch only needs one pad connected to a signal, and their internal connection is designed for an entirely different purpose. It’s intention is to be able to easily design keyboard matrices on cheap single sided FR2.
And for this, there is only one answer:
Connect all 7 pins to your GND plane. There are 7 GND pins for very good reasons. If you are confused about this, then do some research into the importance and use of GND planes.
In my youth, when I was etching single sided PCBs in the bathtub, I even used the two pins to bring GND from one side of the board to the other… Meanwhile I know it better 
Thank you all for your suggestions and comments.
It helped me a lot.
Even though I have an M.Sc. In electronics, I have not used it a lot.
There for I am a bit of a newbie in PCB design.
