How to cut the "T" part of a T-slot using cnc: jog function or tool path?

I would like to add some t-slots to my spoilboard. I know it's best to create the dado first (I have a 1/2" shank Rockler t-slot bit, so I have to anyway), so I'm comfortable with the idea of creating a 3/8" wide dado first.

But since the t portion is at the bottom of the channel (2nd operation), how do I program the t-slot, say if I want the t-slot at 1/2" depth below the top of the spoil board. I would like to start with the y line at x=3 (inches) and y=0.

I hesitate, because I am imagining, since this starts at the perimeter of the spoilboard, that the bit would start spinning, and the spinning t-slot will create a key-hole look at the beginning of the channel as it moves to the depth before it starts its y movement following the channel, and I want a clean look to the spoilboard.

Should I set the depth to measure from the "bottom of Z" versus from the top of Z in Aspire?

Can I just set the depth and location by manually jogging the spindle, then start it spinning outside the perimeter (x=3, y=0), and then Jog it through the end of the channel (x=3, y=24, Desktop MAX)?? i.e., can I use the jog functon of SB3 to cut?

My hand router is the Bosch Colt which only accepts 1/4" shank, otherwise I would have just used it freehand to run the t-slot bit after the dado was created.

I did not want to spoil my spoilboard. Thank you.

I set my material to be 2 inches bigger than my table. I made my lines 2 inches longer to match the material size. I drew a line and used the array to set the spacing I also went in and did a node edit to change every other lines start point. I have cut a lot of special slot wall using this method. Yo have to be out side your material. I cut the dado then another file with the slot cutter set at full depth and in your tool data base set the slot cutter pass depth deeper than your actual cut so it will only make one pass. Hope this helps

Don't use the jog command, use a slower move speed setting in your console if you're going to do it that way. More importantly, do you have enough over travel to start outside the perimeter of your spoilboard? It will be too easy to over travel and either hit the limits or the hard stops and loose steps. If you have enough allowance, draw it up in Aspire using one line that is say 1" past the perimeter. Linear copy the needed number of slots, change the start node of every other one and toolpath ON the line at the needed depth using left to right or shortest path order. You'll essentially have a zig zag toolpath. To make a even more efficient toolpath, instead of changing the start node, connect the lines at the ends to make one continuous path so that the z axis doesn't lift at each end. Z at surface.

Edited....What Jerry said. ;)

plus must of the slowing bits I use have cutters on the shaft so it is a one tool job. I just cut some for a commercial job that has aluminum inserts they are 1" wide. cut them in 3/4" apple ply one pas .75ips will I use a profile pass with a .02 wide rectangle and cut on the line so it cuts both directions.

Thanks. Is there a way to view my hard stops, limits for over travel in the SB3 Editor, or do I manually jog the spindle until I get a warning or it stops? I did not see a settings overview in the editor, it just seems to be a routine it wants you to do if you want to make changes. My spoil board is 24x36. Thanks.

OK, I was finally able to do it. I found the over travel limits by manually moving the spindle by 0.1 inches per move. Outside of these limits, I got the ugly sound. x range was -0.7 to 37.4; y range was -0.45 to 25.2; z range was -.4 to 4.45 (what happened to the advertised range of 5.5 for z?).

I made test cuts clamping a 2x4x24 scrap fir to the spoilboard. Then I was stymied when unable to cut the T-slot bit into the spoil board until I realized I hadn't checked the lower limit of Z. Eventually I got it worked out. I made the material board larger than the actual spoilboard so the T-slot bit would clear the edge coming into the spoilboard. Thanks all for the guidance and what I needed to know. It feels good to make progress.