About Layer Display
Use the Layer Tree to view layers in a part or assembly, view items assigned to a layer, and control how layers are displayed in the model. After you change the layer display status to save your changes, on the View tab, click the arrow next to Status and then click Save Status. If you make further changes to the display status after you save it, you can revert the display status to the saved status by clicking Reset Status.
Hiding and showing layers do not affect model geometry, because these functions only affect features that do not affect mass properties, such as datum planes, axes, and coordinate systems. You can select datum axes that are created with geometry to add to layers either graphically or using the search tool.
You can set the display status of a layer to one of the following:
Shown Layers—(Default) Displays the selected layer.
Hidden Layers—Hides the selected layer.
Isolated Layers—Displays the selected layers and treats all non-isolated layers as hidden.
Layers Shown in Hidden Line—(Assembly and Manufacturing mode only) Hides the components in the hidden layers according to the environment settings for hidden-line display. Other items on those hidden layers are not affected. The rules are as follows:
Environment Setting for Line Display
Hidden Layer Component Display
Hidden Line
Hidden Line
No Hidden Line
In Assembly mode, if you set a specific layer or layers to Isolate, Creo Parametric hides all components. In addition, Creo Parametric hides all other items that are assigned to any non-Isolate layer.
In Assembly mode, if you have components on layers that you subsequently set to Hide,  Creo Parametric hides all nongeometry items (datum planes, datum axes, feature axes) even if they are also on the displayed layers.
In all other modes, if you set a specific layer or layers to Isolate,  Creo Parametric also hides all other layers. However,  Creo Parametric continues to display items that are not assigned to any layer.
You can hide the following types of items in any modeling mode (such as Part, Assembly, or Manufacturing):
Datum features, such as planes, axes, curves, and points
Feature axes, such as the axes for holes on the layer
Cosmetic features
Isolate has priority over Hide. Therefore, if a member is on two layers, one set to Isolate and the other set to Hide, the member is shown. However, if a feature consists of several entities (for example, datum curves), individual entities are not shown if the entire feature is in a layer that is set to Hide, even if the entities themselves are in layers that are set to Isolate.
The only features on a layer that layer display operations affect are datum and surface features. Solid geometry is not affected. For example, in Part mode, if you put a hole on a layer and hide the layer, only the datum axis of the hole is hidden. You can hide the hole itself only by suppressing it directly or by suppressing its layer. The only exception to this rule is that, in an assembly solid, you can hide components.
If you add a new member to an assembly, and a default layer for it does not exist, Creo Parametric does not automatically add it to an existing layer. If a layer in the assembly is already set to Isolate when the member is added, the new member is not shown until you either add it to a layer that is explicitly isolated and repaint the display or clear all the isolated layers. In the latter case, which is the recommended action, all the members of the assembly are shown.
In Assembly, Show affects the level of the member and levels above it; Hidden affects the level of the member and levels below it.