How to create soldermask at pins in APD+ and set up soldermask-to-soldermask spacing DRC

When I try to create a soldermask for pins of BGA or DIE pad using the Create Bond Finger Soldermask command, I cannot choose the Pins object in Find Filter. I can choose only Finger and Vias. 

How can I create soldermask at pins in APD, and how can I set the DRC for the soldermask-to-soldermask spacing for the pin?

Follow the steps given below to create soldermask at pins in APD:

1. Open Allegro Package Designer+ and go to Setup > User Preferences

2.Enable the icp_soldermask_allow_pins variable by going to Ic_packaging > Early_adopter.

3.To create soldermask for pins, go to Manufacture > Create Bond Finger Soldermask.

4. Choose Pins in the Find Filter window.

5.Select the pins to create soldermask. To have an option for checking soldermask spacing, change Class/Subclass in the Options pane from Substrate Geometry – Soldermask_Top/Bottom to Component Geometry – Soldermask_Top/Bottom.

Follow the steps given below to set up Soldermask-to-Soldermask spacing:

1. Go to Setup > Constraints > Modes

2. In the Design tab under the Soldermask section, set the Soldermask to soldermask DRC value and enable the DRC. 

3.Check the SOLDERMASK_SPACING DRC created in the layout.