I assume you mean G68, not M68?
When you rotate the coordinate system, you also need to offset it. Let's assume you rotate 90 degrees clockwise. What was 1 inch +Y will now be 1 inch +X. Also, if you touch off front-left before rotation, that 0,0 will now be back-left after rotation.
What's extra annoying is that rotation happens AFTER all offsets, so if you want to offset by 1 inch positive Y, you have to un-rotate that offset in your calculator (in the previous example, Y+1 becomes X-1 after un-rotating) and then add that offset to your G54 or whatever, so that it then becomes a Y+1 after the rotation.
Here's another option:
Open your G-code file, and save a copy (you know, for backup purposes!)
Now, for every line, where you see an X value, you change it to the same value, but negative, in Y. And wherever you see a Y value, change it to the same in X. Where you see I, make it negative J, and where you see J, make it I.
This will manually rotate the entire coordinate system. You can verify it in your tool path preview program.
Example:
G0 X5 Y2
G2 I1 J2 X6 Y3.732
This turns into:
G0 Y-5 X2
G2 J-1 I2 Y-6 X3.732
Making three parts manually requires more editing, but at this point, it's just copy-and-paste.
Find each tool change. Copy the code after the tool change until the next tool change, and paste it two more times.
Now, right after the tool change, Add a G54 line. Before the first copy, add a G55 line. Before the second copy, add a G56 line. Do this for each tool section.
Now, when you touch off parts, you have to touch them off three times; once for G54, once for G55, and once for G56. Then, when you go, the mill will cut all three parts, each based on their individual touch-off.
Luckily, rotation happens AFTER work offset, meaning it rotates around your work offset zero, which means that you don't need to do anything more to rotate the program than what you already did above.