Part Conversion Warnings siemens NX

Cavity Milling operation under a geometry group with defined trim boundaries will inherit trim boundaries. The tool path may be different.In releases prior to NX4, Cavity Milling operations used trim boundaries from the boundary section on the More page. This was inconsistent with Zlevel and Area Milling, which have trim boundaries in the geometry section. In NX4, trim boundaries are in the geometry section instead of the boundary section. This is consistent with the other operations, and allows trim boundaries to be inherited from a geometry group.

During part conversion, any trim boundaries in pre-NX 4 Cavity Milling operations are moved from the boundary section to the geometry section. The following table shows the effect of this change.

For the last case, the resulting tool path may be different from before NX4, because the trim boundaries are no longer ignored. In this case, you will see the above warning on part conversion.

Projection vector is obsolete. It is different from tool axis. The tool path will be different. As of V11.1, projection vectors are not user definable in Planar Mill. If there is only a slight difference between the projection and tool axis vectors, the system will set the operation Arc Output to None and not generate a warning. This prevents warnings from being created in cases where the projection vector was used to prevent Circle Records from being generated.

Material side of boundary and cut direction may be incorrect. The tool path may be different. The system usually displays this message with the PROJ_DIFF_TLAXIS_911 message. In previous versions of NX, if the projection vector was opposite the tool axis vector (this often happens during mirror translations), the output normally expected was reversed. You could correct this by flipping the projection vector and/or changing the cut direction or material side. Because of this, removing the projection vector makes the output uncertain.

Boundary may not be correct. It has spline member with extension along tangent. The tool path may be different. The system displays this message for operations in which the system extends splines to fill in a boundary gap. Prior versions use a line tangent to the spline as the extension. The new method is to use the splines “natural” extension.

Blank plane is obsolete. Its normal is different from tool axis. The tool path may be different. The system ignores the blank plane if the tool axis is not perpendicular to it. All the stepping passes needed to move the cutter from the blank plane to the floor plane will be missing. If the tool axis is perpendicular to the original blank plane, the system redefines the part boundary to be where the blank plane was. No warning is needed because stepping requirements are maintained.

Clearance plane normal is not parallel with tool axis. The tool path may be different. In previous versions of NX, the tool moved to and from the clearance plane along the clearance plane normal. The new method is to move the tool to the clearance plane along the tool axis.

Because Accept Drive Position option is obsolete, this operation may not convert properly. The Accept Drive Points option in Surface Contouring is no longer a valid option. Operations flagged with this message usually need to be reworked.

This operation involves trimmed surfaces being re-parameterized, please edit the operation. The new surfacing modules recognize trimmed surfaces and the method of reparameterization has changed. In many cases, the path is modified but the coverage is acceptable. This, however, is not always the case, so operations with this message need to be checked carefully.

The tool position between FROM & START points may be different from pre-V10.4 releases. Prior to V10.4, the tool moved directly from the From Point to the Start Point. Now the tool moves from the From Point to a point directly above the Start Point on the Clearance Plane and then to the Start Point.

This operation is converted from a Parameter Line operation, please edit and generate to examine the tool path. The system displays this message in all Surface Contouring operations which have been converted from Parameter Line machining operations.

The Feedrate Compensation for Corner Control will not be available in the converted operation. The system displays this message in Surface Contouring operations which have been converted from Parameter Line machining operations only when applicable.

The Fillet for Corner Control will not be available in the converted operation. The system displays this message in Surface Contouring operations which have been converted from Parameter Line machining operations only when applicable.

The Slowdown for Corner Control will not be available in the converted operation. The system displays this message in Surface Contouring operations which have been converted from Parameter Line machining operations only when applicable.

Invalid points (either avoidance or tab points) were encountered and deleted. The system displays this message when it finds an operation containing invalid references to point entities. In these cases, you need to remove the reference from the operation. This can happen to tab points or avoidance geometry points.