How Should CNC Precision Machining Be Arranged for Multi-Cavity Molds?

The difficulty in CNC machining of multi-cavity molds is not "milling out each cavity," but making every cavity identical. A single-cavity mold only needs to control absolute dimensional precision, while a multi-cavity mold must additionally control the relative consistency between cavities—cavity center distance, coaxiality, depth difference, and profile tolerance. If any one of these accumulates deviation, the molded products will show weight differences, wall thickness differences, or even fail to be interchangeable during assembly.

This consistency requirement determines that CNC machining of multi-cavity molds cannot be arranged on the basis of "machining one cavity at a time." Instead, synchronous control must be implemented at four levels: datum, clamping, programming, and inspection.

First, Unified Datum Is the Prerequisite—Design Datum and Process Datum Must Coincide

In multi-cavity mold machining, the most problematic step is often not the cutting itself, but the choice of datum. If the design datum on the drawing is the product centerline or parting surface, while the operator uses the mold plate edge or a process hole as the datum during machining, the deviation between the two will directly translate into positional deviation between cavities.

The correct approach is: establish a "process datum surface" or "datum hole" at the mold design stage and carry it through all cavity machining and inspection. This datum is usually chosen as the guide pin hole system of the moving and fixed halves or the locating mounting surface of the mold plate. During machining, all cavity modules are clamped uniformly to this datum, and during inspection, measurements are also referenced to this datum. Coincidence of design datum and process datum is the first step in eliminating datum conversion errors.

For high-precision scenarios such as multi-cavity bottle preform molds, the precision requirement for unified datum is even higher. Some practical solutions require all cavity modules to be uniformly referenced to the mold locating mounting surface, completing the milling of the cavity surface and gate in a single clamping, avoiding the geometric tolerance deviations caused by multiple clampings.

Second, Clamping Strategy Determines Inter-Cavity Deviation—Prioritize "One Clamping, Multiple Cavities in Synchronization"

The greatest taboo in multi-cavity mold machining is "machine one cavity, release the fixture, then clamp and machine the next cavity." Every re-clamping introduces new positioning errors. After machining several cavities, errors accumulate cavity by cavity, and ultimately the center distance deviation between adjacent cavities may exceed 0.01 mm.

A reasonable clamping strategy is to complete the machining of multiple cavities in as few clampings as possible. If the machine table is large enough, multiple cavity modules can be clamped simultaneously on the same base plate, fixed with a unified positioning system, and all cavities can be rough and finish machined in one pass.

For cases where the number of cavities is large and cannot be completed in one clamping, a dedicated fixture combined with an indexing plate can be used. Some patented solutions design a dedicated fixture with "one surface, two pins" positioning, combined with an indexing plate to achieve non-repetitive clamping positioning, improving efficiency while ensuring machining accuracy. Similar ideas exist in half-mold machining: placing the mold into an eccentric sleeve fixture and using the high-precision positioning characteristics of the eccentric sleeve to machine cavities at different positions by rotating the fixture, ensuring the coaxiality of cavities at both ends.

Another approach worth noting is the datum-first machining method. Before formally machining the cavities, first finish machine a "datum surface" or "datum hole," and all subsequent cavity machining uses this datum for tool setting and inspection. Some patented solutions, in machining the parting surface of large injection molds, first pre-machine a datum surface in the near-cavity area, then use it as a datum to machine the far-cavity area, controlling the machining sequence and allowance of the two areas to ensure height consistency across the parting surface.

Third, Programming Strategy: Subprograms Are the Core Tool—Incremental Programming Makes Shape Independent of Position

In CNC programming for multi-cavity molds, if each cavity is programmed with its own separate program section, not only is the programming workload large, but it is also easy to create inconsistencies in cutting parameters between cavities. A more reasonable approach is to use subprogram programming: write the contour machining path of a single cavity as a subprogram, and have the main program only call the subprogram and specify the coordinate position of each cavity.

The key technique is to use incremental programming (G91) for the subprogram. This way, the contour shape programming is independent of its absolute position on the mold. The same subprogram can be called by all cavities, and only the starting point coordinates of each cavity need to be given in the main program. This method not only greatly shortens programming time, but also ensures that the tool paths and cutting parameters of all cavities are completely identical, eliminating inter-cavity differences introduced by programming at the source.

For cases where the cavity shape is complex and requires multiple operations (rough machining, semi-finish machining, finish machining), a separate subprogram can be written for each operation, and the main program calls them in sequence. The same operation for all cavities uses the same subprogram, ensuring completely identical cutting conditions.

Fourth, Precision Control: Shift from "Inspection After Machining" to "Compensation During Machining"

In CNC machining of multi-cavity molds, if you wait until all cavities are machined before conducting CMM inspection, there will be no allowance left to correct when problems are found. A more effective approach is to introduce error detection and compensation mechanisms during machining.

One feasible solution is: after finishing every 1-2 cavities, pause machining and use the machine's online measurement system or a CMM to inspect the key dimensions of the machined cavities, compare the measured errors with theoretical values, and correct the tool compensation parameters or machining coordinates for subsequent cavities according to the deviation direction. This way, even if the tool wears, the wear can be offset by cavity-by-cavity compensation, ensuring that the final dimensions of all cavities fall within the same tolerance band.

For scenarios with many cavities and obvious tool wear (such as slow wire cutting of multi-cavity molds), the wear amount of the tool or electrode can be measured after rough machining, and then the wear compensation value can be added to the finishing subprogram. Some solutions recommend inspecting the machine's positioning accuracy after finishing every 1-2 cavities to avoid error accumulation.

Fifth, Final Inspection Must Be Conducted Cavity by Cavity—CMM Is the Standard Means

After multi-cavity mold machining is completed, acceptance inspection cannot just measure "one cavity as representative of all cavities." Every cavity needs independent measurement of key dimensions: cavity diameter, depth, center distance, coaxiality, and profile tolerance.

A coordinate measuring machine (CMM) is the standard means. Import the CAD model of the mold cavity into the measurement software, measure the key control points of each cavity, compare the measured point cloud with the theoretical surface, and generate a color map to visually display deviations in each area. For multi-cavity bottle preform molds, industry practice requires cavity diameter deviation to be controlled within 0.003 mm and geometric tolerance not to exceed 0.002 mm.

Inspection data should also be used for reverse correction. If a cavity's dimensions are found to be close to the upper tolerance limit, and subsequent polishing or EDM machining is still to be performed, the allowance for subsequent operations needs to be adjusted to ensure the final dimensions will not exceed tolerance. If deep cooling treatment or stress relief operations are still to be performed after cavity machining, corresponding deformation compensation must also be reserved.

Ultimately, the Core of CNC Precision Machining for Multi-Cavity Molds Is "Synchronization," Not "One by One"

The machining logic of a single-cavity mold is "make this cavity as accurate as possible"; the logic of a multi-cavity mold is "make all cavities equally accurate." The former pursues absolute precision; the latter pursues relative consistency.