Drawing display style changes when I open the file

Datum Display Filter settings are global for the whole Creo session, so you can't disable them by default just for drawings and leave on for other modules (like Part or Assembly). When it comes to displaying datums, you just need to remember to turn them off in the drawing or set them to be off by default for the whole Creo.

As for displaying drawing, you have defined drawing view display as "Follow Environment", so the geometry display style in the drawing will match any setting you currently have for the whole Creo session. You need to go view properties, select View Display category and change Display style from "Follow Environment" to some other setting. That way your view will retain specified display style.

Also, if you want to define a particular display style for any drawing view you create, go to File > Manage > Drawing Properties > Detail Options and set model_display_for_new_views to other value than follow_environment. That way any new view you create in that drawing will use display style you defined through that option. And if you want to keep this setting as default for all drawings, you need to edit your .dtl file and change the same option (model_display_for_new_views) there.

I would also add that you should put the model datums on layers.  Then, in the drawing, hide the layers and save the layer status.  This will keep all of the datums hidden.