KB: Cannot delete Layer from Layerstack

This article describes several scenarios in a Pcb document that can prevent layer deletion in the Layer Stack Manager.

Starting in Version: 19.0
Up to Version: Current

Solution Details

Problem: Layer cannot be deleted in the Layer Stack Manager, the option is grayed out.

There are several known scenarios and corresponding solutions discussed here:

1. Stack symmetry lock for a non-symmetrical board.

2. Limitation in Altium Designer pre 20.1 for adjacent core / prepreg..
3. Minimum 2 signal layers constraint
4. Other unexpected scenarios

Solution 1 - Stack Symmetry:

In some cases, possibly caused by importing or copying / pasting from other boards, can cause layer creation resulting in a non-symmetrical board stackup.

In the Layer Stack Manager Stack Properties Panel, there is a symmetry option. If this option is enabled and there is a non-symmetrical stack, this will prevent layers from being deleted.

To remedy in this situation, uncheck the symmetry checkbox which will allow deletion of the layers. When the symmetry option is enabled, a check for stack symmetry is performed, but certain board level operations can bypass this and create signal / plane layers.

Solution 2 - Layer Order Limitation:

In Altium Designer 19, there was a limitation that did not allow two

cores to be stacked together. This results in an error state and does not allow the layer to be deleted. This is resolved in our Altium Designer 20.1.7 release.

As a workaround to fix the stack in AD19:

1. Review all the layer names and rename any layers to be sure they are unique.

2. Change the Type of one of the adjacent cores from Core to Prepreg.

The improvement in Altium Designer 20.1 was #36545 .

There are also some other, more obvious constraint enforced such as not allowing adjacent two signal/plane layers (removal of core/prepreg in-between)

Solution 3 - Layer Count Limitation:

 Maximum of 32 signal layers and 16 plane layers , down to the minimum of 2 signal layers are allowed. For single-layer board, such as one-sided flex cable, please refer to another article Single-Layer-Board .

 Solution 4 - Other Unexpected Scenarios:

The stackup may fell into some unexpected state where a layer cannot be deleted possibly due to incremental changes and updates across multiple Altium Designer versions where varying limitations/constraints are enforced. While we do our best to maintain the upward/downward compatibility, there may be some scenarios that are not accounted for. One solution identified in such case is to save the stackup externally (File » Save As...) first and then to reload it (File » Load Stackup from File...).