why is there still no tool for putting a work plane between two surfaces?

Relax, look this two options.

Using offsets planes.

• Select a plane parallel to the desire one
• Click Plane
• Enter the offset value desire

That value (for what I can see in your pictures) is constant, so you can repeat this process over and over again, starting a new plane from the last created. You just need to measure the middle point between the two surfaces once, and add it to the offset of the new plane. You can even use a the relation option for that.

Using the Pattern feature

• Using the previous method create a plane placed only and just only in the desire location, the middle point in your case. This plane must be parallel to the plane RIGHT, LEFT, or TOP plane, depending of the orientation.
• Click the new plane
• Click pattern
• In the dashboard, change the type to direction
• Click the plane that is normal to the direction that you want to create the pattern (This plane is parallel to the previous one, and must be RIGHT, LEFT or TOP plane depending of the orientation)
• Modify the number of planes and the offset distance
• Click OK

If there's more than one use in a part, you can copy the group and paste with advanced references. It may be amenable to a UDF.

You can also create the plane offset from one of the surfaces and drive the value by a relation based on a measurement feature between the two surfaces.

If the problem is with just one plane

• Measure the distance between the edges using the measure tool in the Annotate tab (let say that distance = x)
• Select an edge of the part, press CTRL and select a plane parallel to the desire one
• Change the rotation to 0 and click ok
• Make an offset plane of this plane using the procedure explain it above, and for the offset distance type x/2

That's all.