How to add symmetric ground reference via in PCB editor 17.4?

Forgive me as I don't get to work with PCI-E. 

But, from an RF standpoint, splitting a diff pair is never a good idea, regardless of bit rate.   You lose common-mode noise rejection, impacting BER, when your coupling spacing is spread like that.

Sometimes, we have ground pour "peninsulas" that stick out that need to be "tacked down" with extra vias.   I can't think of a benifit of that via.

And, adding gnd vias close to the device increases risk of impedance discontinuity from your signal nets to any ground via. 

Is your signal to ground spacing trace to via pad about 1.5 to 2x your dielectric thickness to layer 2?

Ground via is used for a return reference for PCIe signal vias. It is advised to have 2 ground vias and due to space constraints, I am adding only one via. 

I forgot about the multiple ground plane problem if you are jumping from front to back.   I.E. need to stitch the ground reference planes together around the transition.

Do you have the high-speed rules license option?  It automates this problem.

We have to avoid causing an increase in self-heating of the board with an impedance mismatch.  To minimize insertion loss, my coworkers design an impedance-controlled transition:  a signal via plus up to four ground stitching vias then validate it using Microwave Workbench.  

We drive repeatability by building a library of thru-hole component for the correct via arrangement for a stackup and add these parts to the schematic.  

It's very low tech but we don't use other features of the Allegro PA-3100 high-speed option to justify that option license (costs more than base Allegro.)   

I have fixed the problem using the "slide" option by selecting the via and the entire line segment of the differential signal. The suggestion of using a thru-hole component seems interesting. I think I have to create a footprint with the via structure. I wish I could add more ground vias, but four ground via is an ideal situation when the board becomes dense. 

I have fixed the problem using the "slide" option by selecting the via and the entire line segment of the differential signal. The suggestion of using a thru-hole component seems interesting. I think I have to create a footprint with the via structure. I wish I could add more ground vias, but four ground via is an ideal situation when the board becomes dense.