Hiya

Sketchucam uses 2 feed rates set on the Parameters Dialog on the second line down
Feed Rate and Plunge Rate
Feedrate is the normal cutting feed rate used for all X and Y moves.
Plunge rate is the vertical rate used for all Z plunge moves, which includes drilling holes and plunging after tabs

So, here is an example of Gcode generated from a simple 50x50mm square with a tab at top and bottom.
I will add some comments to the lines to explain what it is doing......

G90 G21 G49 G61 G17 I use metric, but the principal applies to imperial as well
M3 S30000
G0 Z5.000
X8.500 Y8.500 start point
G1 Z-6.300 F1000 feed Z down at 1000mm/min = 'plunge rate'
X31.500 F2000 cut X to the start of the tab at 2000mm/min = feed rate
Z-3.000 move up onto tab
X38.500 cut top of tab
Z-6.300 F1000 plunge down after tab at plunge rate
X61.500 F2000 cut in X again at feed rate
Y61.500 next moves will keep 2000mm/min feed rate
X38.500
Z-3.000
X31.500
Z-6.300 F1000 until here where rate is changed for the plunge
X8.500 F2000 and back to 2000mm/min
Y8.500
G0 Z5.000 retract at rapid rate
G0 X0 Y0 (home)
M05
M30

now, if your Gcode looks like that but does not cut like that the problem is the controller itself, or possibly the software feeding the Gcode to the controller (some of them try to 'simplify' the Gcode). Try the Universal Gcode Sender instead since it does not alter the Gcode that I know of. If it still cuts slowly, maybe GRBL is not set up to cut any faster? maybe you can post the GRBL setup values so we can cross check for you.

@kram242 (our website host) is quite fluent with GRBL and has been doing a lot of testing lately and has not noticed this slow feed after plunge that I know of.

if your Gcode does not look like that then you need to make sure you have the latest version installed
(1.2a at the moment). if you do have that, then you need to post your drawing and your Gcode in a reply here so I can see if I can can figure out what is wrong. we are just about to release a new version so if something needs fixing I'd like to know soonest (-:

BTW you only need to specify a slower plunge rate if your material is hard enough to warrant it. if your machine and tool bit can handle plunging at the usual cut rate, then by all means use the plunge rate = feed rate. for example, if you are cutting balsa wood with a 2 flute router cutter then it should be able to clear chips fast enough to plunge at normal cutting feed rate, but a 4 flute will probably not so you will need to plunge slower or maybe use multipass to allow it to clear the chips.

in plywood the chips will likely be bigger and harder to clear, so even the 2 flute may struggle unless moving slowly.

Note that you can use the Tool Profile save and load buttons to save feed speeds for tools, and later reload them easily. This saves having to remember to set the speeds for a particular tool.

Also, the Tools|Phlatboyz|Options menus allow you to set various defaults that will be the settings used for any new drawing.

Please hit the big blue question mark button on the SketchUcam toolbar and read the help. You will learn a lot of tricks and techniques for using SketchUcam, try out one at a time just to see what happens (-:

looking forward to figuring this one out...