Most designers and engineers utilize "Geometric Dimensioning and Tolerancing" (GDT) practices. Below are some considerations related to the application of these practices to the machining of aluminum castings. It is TAC's experience that some explanation of the impact of the use of GDT on parts to be cast and subsequently machined is useful. A datum feature must be an actual feature of a part. Center lines and center planes are theoretical. They do not exist as features on an actual part and, therefore, may not be used as datum features. 

A datum is selected on the basis of its geometric relationship to other features and the functional requirements of the design. For mating parts, it is usually desirable to select corresponding features on each part as datum features to ensure proper interface in assembly. Datum features must be readily discernible on an actual part, be accessible and be of sufficient size or extent to permit their use for manufacturing and inspection activities. 

A casting is typically a framework to hold together places to fasten other components. The cast surfaces are generally secondary in accuracy requirements to the areas machined (threaded holes, reamed holes, milled slots, grooves, surfaces). This leads to the need for two datum reference frames . Selected datum features of castings may be used temporarily for the establishment of machined surfaces to serve as permanent datum features. Such temporary datum features may or may not be subsequently removed by machining. Permanent datum features should be physical elements not appreciably changed by subsequent machining operations. 

Datum targets, as applicable on cast or machine surfaces, should be chosen with the following points in mind whenever possible: be a feature on the part; be accessible; be capable of being clamped properly and not be located on cored surfaces. Datum targets in any one datum plane should not cross the mold parting line There are many good reasons, as outlined in ANSI Y14.5-1982, for proceeding in the above manner.

Additionally, good machining practices dictate the need for part rigidity during machining which, in turn, requires good fixturing and clamping. Clamping should be done on the ABC datum reference frame targets and in such a manner as to machine as many of the required surfaces as possible. This reduces the number of setups required to complete the part and helps to reduce the amount of variation from casting to casting. Clamping must be sufficient to hold the part in place while resisting machining forces, but not so tightly or on a surface that will cause deflection. 

This leads to another major area of concern - true position callouts. Designers understandably want the highest quality possible in the parts they create. This sometimes leads to unrealistically small true position callouts on a drawing. 

Experience and observation have shown that a number of factors impact on the ability to hold true position: 

• Deflection caused by poor clamping circumstances, flimsy casting structure, machining forces and thermal effects (both the heat treatment of the casting and the ambient temperature conditions during machining versus those in which the casting is used). 

   

• Machine tool capability: a manufacturer may claim repeatability of ±.0002 inch. This may well be true at the time the machine tool was built and under "lab" (non-machining) conditions. Actual manufacturing conditions and age of the equipment can erode this capability considerably. 

   

• Post-machining operations such as plating, anodizing and painting if not properly controlled or anticipated will affect true position (among other things). Consequently, a true position callout of .002 inch or smaller is typically difficult to achieve.  With all of the above in mind, a callout of .005 inch for true position will generally be a far more practical and economical value to use. 

Definitions: (Taken from ANSI Y14.5M-1982) 

Datum - A theoretically exact point, axis or plane derived from the true geometric counterpart of a specified datum feature. 

A datum is the origin from which the location or geometric characteristics of features of a part are established. 

Datum Reference Frame - A system of three mutually perpendicular datum planes or axes established from datum features as a basis for dimensions for design, manufacture and verification. It provides complete orientation for the feature involved. 

Datum Plane - Theoretically exact plane established by the extremities or contacting points of the datum feature (surface) with a simulated datum plane (surface plate or other checking device).

 Datum Feature - An actual feature of a part that is used to establish a datum.

 Datum Target - A point, line or small area specified on the part to establish a datum. 

True Position - A term used to describe the perfect (exact) location of a point, line or size feature in relationship with a datum reference or other feature. 

The suggested hierarchy and identification of datum reference frames and their constituents, as used at TAC, are as follows: 

"A" datum plane - The primary datum plane consisting of datum targets A1, A2 and A3. 

"B" datum plane - The secondary datum plane consisting of datum targets B1 and B2. 

"C" datum plane - The tertiary datum plane consisting of datum target C1.

 "A", "B", "C" (ABC) datum planes are mutually perpendicular, are assigned to or utilized with cast features only on an unmachined or machined casting and may be temporary. 

"D" datum plane - The primary datum plane consisting of datum target D1, D2 and D3. 

"E" datum plane - The secondary datum plane consisting of datum targets E1 and E2. 

"F" datum plane - The tertiary datum plane consisting of datum target F1. DEF datum planes are also mutually perpendicular, are assigned to or utilized with machined features on a machined casting only, are permanent and are typically assigned a "start" dimension corresponding to cast datum features. 

Thompson Casting is ready to help any customer in understanding how the above concepts affect the design, manufacture and cost effectiveness of their parts. If there are questions to be answered or issues to be resolved, please contact our Engineering Department. 

A "DATUM" is a feature or group of features of a part, selected for use as a base from which other features or points are located within specified limits. To achieve consistency in the manner in which measurements are made in all stages of production; i.e., pattern making, casting layout, tooling layout, etc., a system known as target points or datum lines, or datum planes has been devised. 

For the purposes of this standard, "target point" and "tooling point" are synonymous. This system relates all significant dimensions to a common reference (datum plane). It is strongly recommended that those points or planes from which inspection and/or machining layouts are started, be indicated on the drawing by symbol or other means. 

Where datum planes or target points are not indicated they shall be selected by the foundry, which will choose surfaces formed by the most stable portion of the mold. Such designations tend to control the accumulation of tolerances in addition to their prime purpose of establishing a common location from which to work. It is preferred that they be surfaces not affected by mold parting. Also, the surfaces at which gates and risers are to be placed are unsuitable as target points as a result of trimming and rough grinding operations. 

Target points should be avoided if possible on cored or tapered surfaces. They should be located close to the extremities of the casting whenever possible to eliminate variations in alignment due to projecting small surface irregularities. 

The designer of a casting, the tooling engineer and the foundry should work together in establishing target points or datum planes because they directly influence casting cost not only from the tooling standpoint but also from the foundry standpoint. 

Fig. 1 Schematic illustration showing the perpendicular relations among the three planes in a system.