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Barnaby wrote:I get an error message “Removing splitter failed”
This is a message from the RemoveSplitter() algorithm that cleans up faces of the residual edges left by Boolean or feature-based operations. This algorithm is implemented in the GUI in 3 different ways: from the Part --> Refine shape menu (creates a new unlinked object, thus should only be used on converted meshes or imported solids), the OpenSCAD Refine Shape Feature and an automatic mode in the preferences.
Therefore, you are getting this message because you enabled "Automatically refine shape after Boolean/feature-based operations" options in Edit --> Preferences / Part Design / General. This message is telling you the algorithm has failed to operate and prevents the Pad from completing.
You can avoid this message by deactivating the auto refine settings then editing the Pad again. But know that doing so in the middle of a model can be extremely disruptive. Your model only contains 2 sketches and 2 features, the results are fine. But doing so on a model with many features and sketches would be catastrophic and break the model. For this reason, even if the auto refine options were implemented on my request, I no longer use them for files shared in the forum. I prefer to use an OpenSCAD Refine Shape Feature once the model is finished.
That being said, it is always best to avoid tangent and coplanar surfaces when applying Boolean operations and PartDesign features.
The problem you are having can be fixed in a cleaner manner if you edit Sketch001 and change the radii values from 37.5mm to a smaller value, for example 37mm. This way, the produced pad will have a smaller diameter than the outer body, this will fix the remove splitter error and you'll be able to pad to exactly 48.000mm.