Create your model the size you want your finial to be in our case we want a width of 14 inches.  The height of the model is the diameter of the blank you want to use * pi (3.14...) which comes out to approximately 12.5.

You need to create a border file first to give the boundaries for the turned section to my program.  This is just a matter of creating a rectangle 14 X 12.5 and centering in the model (which creates a box outlining the model). Create the Machine along vectors toolpath as the following screen depicts.  Toolpath should be created at zero depth.

Following is from the picture Denver posted.  I used node editing to create the profile bottom vector and mirrored the vector and moved to the 4 inch diameter guideline to show what the turning should look like.

Now we need to create a mirror center vector to create a 3D model to put our reeds on using a 2 rail sweep.

Notice the following vector has the left and right ends joined and that they go down to zero.  This is needed to create the 3D model properly.

Following screen is of the 2 rail sweep.  We select top (left) and bottom (right) rails and add the profile vector as the cross section and calculate.

We get the following 3D pattern from the 2 rail sweep.

Now we need to define the material in order to get the reeds at the right depth.  Set the depth for the finial at 4 inches.

Following screen shows the material defined.

Now we go back to the 2D view and create a line vector at x=0 on the profile where we want the reeds to carve.  We wanted 24 reeds so we divided 12.5 by 24 to give us .5208.  Do a block copy of 24 using a gap of .5208 to get the vectors as in the following screen.

Now we go to the vectors drop down menu and select create feature and center line engraving for the reed vectors selected.

Give the feature a depth of .2 and name it Reeds.

Following screen is the Feature Machining option of ArtCAM.  Bring in the Reeds feature select a bit and calculate.

The reeds toolpath is created to follow the contour of our relief.

Following toolpath is created for simulation only and not needed for the actual turning.  It is just a machine relief toolpath of the entire relief.

After running the machine relief and the reeds feature toolpath we get the following simulation.  Notice they are straight at the moment but because of the curve of the turning they actually bend inwards when turned.

Now we need to create the indexer profile using the bottom profile vector created earlier.  No vectors joined on the right or left going to zero for this one.  We go to machine along vectors toolpath and set the finish depth at the vector height which happens to be 1.665.  The stepdown value of the cutter you select is actually the amount of material removed each pass so .2 is probably good most of the time. Calculate.

We get the following representation of the toolpath.  Notice it goes down to the depth of the inside of the turning.  The program converts the Y values to Z values to accomplish the turning.

Next save your toolpaths as Shopbot(inch)(*.sbp).  That will complete the ArtCAM portion of this project.

See setup procedures if you have not done setup.  The one item that really affects the turning and time is the stepover setup value.  I tried .1 with a .5 ballnose first and it ran quite quickly but had lots of larger lines in the turning.  I chose .01 next but after running the converter it showed that it would run 11 hours or so. Compromised at .05 which said 2.9 hours I believe - but it's totally up to you.  I noticed on the final output with ballnose bits the square edges are not appearing.  Possibly one could create the model with a little extra material in certain areas and run an endmill along those areas to remove and square the edge.

Anyway select 1 section - round type - 1 file and select the border file to start the converter process and setup the boundaries.

We want to overlay the border file with our profile file so select yes on the overlay.

Select the profile diameter when asked.

Select the profile file. 

Next select a round section for the reeds toolpath.

Select the reeds file.

When asked to overlay after the reeds file click on the no button and you will be taken to the following screen asking for the output file name.

To calculate the safe distance to rise in Z the program needs the bit length from the collet to the end of the bit.  Enter as close as you can. with the existing values. It will ask for each file you entered.  I usually put the bit size in the file name someway.

Last screen gives you the dimensions of the turning.  If they are what you were expecting click done.  Go edit the output file and see if it looks appropriate. Be cautious when running new files.  Make sure your model toolpaths do not have a severe downward spike somewhere which would drive the Z into the material.