Ok so I did some Testing and in short to answer my own Question, Yes it will work.

Those working with V-Carve Inlays understand that if we set our Start Depth at .1 and Flat Depth at .1 as Seen below

The CNC machine is going to ignore the first .1" of our Material and Say if we set our “Pass Depth” to 0.05" The bit will be plunged down 0.15" into the Material before cutting. With our parameters set above it would mean that 2 Passes would be made and the result would be the surface depth at 0.2" deep.

Working with Wenge; I do not want to cut down 0.2" into the surface let alone 0.1" due to breaking bits, but rather take smaller passes so This is how I achieved it.

I first did a Pocket cut, The end result needed to be 0.2" Deep so I did this with 4 Passes using a 1/4 EM DC, and 1/8" EM DC bits.

This allowed for roughly 0.05" passes, while it does take longer my Bits Survived and cut nicely

Now in the Next Step I found the Areas inside the Logo that would use a larger Clearing bit, and i applied the Same logic going after those Areas as well with a Pocket Cuts at 0.2" Deep in 4 Passes with the 1/8" & 1/4" Bits.

These Tool Paths were Sent to the CNC and sure enough everything cut smoothly and no bits breaking.

Now finally to What my initial Question Was, I know i need the V-Carve to be .1 Start Depth & .1 Flat Depth, I know I don’t Want The V Bit To Plunge that far into the surface so What if I try .05 SD & .05 FD, first then running the right tool path will the Shape still come out the Same?

Here is the Results from the First Cut:

*Notice inside the nose and brim of hat it has an abrupt stop, that is 0.1" below the surface as we told the bit to start at .05" below the Surface (Z) and it cut down from there .05*

With the Final Pass we don’t need to Touch anything or Home The z, I simply ran the Next pass at the desired 0.1 Strat Depth & .01 Flat Depth resulting in the carve being at the final 0.2" depth.

*As you can see the results came out excellent and look exactly as they should but here is the Question; ***Will it Fit Into the Female Piece!?!?!**

So I set the Female Piece at 0.0" Start Depth and 0.15" Flat Depth, The Pass Depth is 0.125" so The Bit needs to make 2 Passes to reach the desired depth, The wood is Walnut so I’m perfectly fine leaving these settings:

Now Time For the Glue up & final Result

As you Can See Everything Came out as Expected with the little details such as the Stars Eyes making their appearance. So as mentioned above to my original Post & Question the Answer is **Yes** for anyone pondering attempting the Same scenario