What you should know about Moldmaking

Steve MacKay
Principle
Wisconsin Mold Builders
Waukesha, Wis.

Edited by Paul Dvorak

Many engineers suffer under the assumption that toolmakers immediately start cutting steel after they receive part files. Not quite. Toolmakers usually devote the first several hours cleaning and correcting the file to make the part manufacturable. In fact, a lot of standard engineering habits unwittingly add hours to manufacturing tasks. If designers knew what goes into moldmaking, they would not create the problems moldmakers encounter, thus cutting most of the wasted time off the entire operation. Here's some of what moldmakers do before cutting steel.

A toolmaker's first task is usually to clean up a part file after bringing it into a CAM system, usually by IGES or a custom translator. They delete unneeded geometry, construction lines, and duplicate surfaces. These frequently show up in part files. Unneeded geometry creates confusion while adding megabytes to file sizes. All of it must be deleted. And the additional work might show up in a new quote, especially if significant problems arise.

Toolmakers then look for missing and incorrect surfaces. Engineers regularly submit part geometry with slits or gaps where surfaces do not quite come together, and triangular holes at the bottoms of inside corners. These are found by shading the geometry and zooming in on suspicious areas. Slits must be geometrically "stitched" together. Missing surfaces must be generated, properly curved with correct tangencies, and dropped precisely into position.

Cleanup usually includes trimming multiple surface extensions back to their intersecting surfaces. Geometry from clients often has lines and planes that penetrate or extend past adjacent surfaces. These must be identified and corrected, ideally for each surface. This kind of cleanup is usually done three or four times when creating geometry for molds.

The process continues by dividing the part's geometry into halves corresponding to the mold tool's core and cavity. This is done by separating all aspects of the part that belong with its inner surfaces (the core) from those belonging to outer or visible surfaces (the cavity). CAM software should do this automatically.

For many parts, customers provide only exterior surfaces and a specification for material thickness. This requires the toolmaker to create the mold's core by offsetting the cavity surface by the specified material thickness.

While most tool-design work is done in surfaces, some interior CAD work on mold cores is best done in solids. Because simple shapes such as bosses and stiffening ribs are geometric primitives, they can be created with primitives more quickly than with surfaces.

Preparation to cutting is simpler when done on a CAM system with a single geometry database for both solids and surfaces. This way, a single database holds all geometry rather than placing solids in one and surfaces in another. Many CAD packages, on the other hand, use separate but "synchronized" databases. The synchronization between them rarely works as promised.

Working on a core highlights a drawback of solid-modeling systems — open volumes. Most solid modelers require watertight volumes to make sure geometry is completely attached where it should be. This is a sensible approach for ordinary machined parts and components which are orthogonal in two or three axes. In modelers that need tightly closed volumes, however, converting surfaces to solids creates severe problems. For one, it's a Herculean computing task. For another, geometric primitives accumulate and files can become unmanageably large. Consequently, creating ribs and bosses for a tool's core is much simpler when so-called leaky solids can be used.

Draft angles are another key part of a mold's core tooling. Surfaces on bosses and ribs are often parallel to the direction of the mold's "pull" when it opens. Unless those surfaces slope gently inward by one or two degrees, parts will stick in the mold.

A next step focuses on inside corners of the cavity and core. To avoid unmachinable sharp inside corners, moldmakers create fillets wherever pairs of curved surfaces intersect. Variable-radius filleting and trimming comes in handy here. Fillets must exactly meet all adjacent surfaces, so their radii may vary across a wide range.

Toolmakers must also search models for unnecessary and inaccurate geometry. To machine efficiently and keep models as small as possible, the mold creation package must identify and delete points (sometimes thousands of them) not needed to establish tolerances. At the same time, the software should let toolmakers quickly detect and repair unwanted sags, flat spots in curves, and humps in surfaces that should be flat.

CAM software should also give users Boolean or algebraic operations. Boolean subtractions work well, for example, when creating geometry for complex stiffening ribs in a mold core. Boolean subtraction is also handy for making graphite electrodes for electrical discharge machines (EDMs). This is called electrode extraction. It is used for producing mold details too small for machining. Appropriate geometry is extracted, turned inside-out, and offset by the EDM machine's specified spark gap. The CAM system must let moldmakers window and extract the detail, modify it as necessary, and download it to a CNC machine.

Additional tasks determine the mold's parting line and create runoff surfaces. A parting line separates the core and cavity halves. On-screen, runoff surfaces wrap around the mold as a flat surface or a gently undulating plane at the parting line.

A good CAM system helps correct a lot of the flaws in submitted geometry. Another way is to avoid the flaws in the first place, for example, by including draft on parts, rather than letting the toolmaker do it. You might also ask your toolmaker whether they prefer to receive models in IGES, STEP, or another format. After all, it is your part we're making.