dimension and tolerance change synchronous between save as drw and the initial one

It's happening because, by default, Creo saves drawing dimensions in the model.  This applies even to driven dimensions created in the drawing.

A way around it is to set the config.pro option "create_drawing_dims_only" to "Yes" when working on one of the drawing types.  This will save created dimensions with the drawing.

Note that this setting does have a few downsides, mostly involving some aspects of using GD&T.

-Doug

Depends on how you've got things set up. If you are showing the model dimensions, the ones used to create the geometry, they will have their tolerances and those are the same wherever you show them.

If you created the dimensions in the drawing, you will still see this behavior if you show them in another drawing because by default dimensions created in the drawing are stored in the model. Their tolerances and appearance will be whatever they were set to last. I.e. if you change a dimension's tolerance in drawing A when you create it, copy the drawing to drawing B and modify it to a different tolerance in drawing B, the change occurs in drawing A, too, since they both refer to the same saved data in the model.

There are two ways I know of to avoid this:

(1) In your config.pro, set create_drawing_dims_only to yes. This means the dimensions you create are stored in the drawing file, not the model. I've not done this, but imagine when you copy the drawing to the customer drawing you can then modify the tolerances and it will behave as you wish.

(2) If you don't want to set the parameter in option (1), you have to create separate dimensions for both your internal and customer drawings. When you copy the internal drawing to the customer one, you'll have to "erase" (not "delete") the ones you want to be different from the copy. Then create new dimensions for them. It's tedious.