Concentricity in Deep Hole Applications
Recent News - February 19, 2014Article on Concentricity – Part Three
by Geoff Ginader
President American Hollow Boring
How straight will the hole be? That is a question that must be considered when planning to produce a deep-hole machined part. The planning process should verify that the boring process can produce the hole as accurately as the application requires without excess processing. This article will seek to inform the reader about the range of properties of form that may be specified and how they apply to manufacture of machined deep holes especially in round bar applications. This may facilitate communication among engineers, purchasing professionals, and manufacturing management. Sound planning and communication will contribute greatly to a positive outcome in terms of parts that meet spec and thus work as intended.
First, consider the simpler case of rough-bored holes. Rough drilling operations generally allow a wide tolerance on drilling, no finish requirement, and straightness considerations are minimal. Very deep holes should allow enough stock to clean up after a worse case runout of .001” per inch. Therefore, a part that is 180” long should allow more that .180” in the bore for clean-up or more depending on the subsequent operations. If such stock is not available, options should be discussed with manufacturing. Options may include drilling the initial hole smaller or specifying finish boring with runout of less than .001” per foot. It is a very good practice to supply a desired hole size and size of the finished ID as well as size of the OD and finish OD size when requesting quote.
When tolerances become tighter and size becomes more critical, it becomes more important to understand the general requirements of straightness or concentricity. To illustrate this, suppose a 4” hole has a .003” tolerance on size and is 10 feet long. Without specific definition on runout, the hole technically should be within .003” in runout. It may be a simple operation to hold a size of .003” round and true within .003” in 6” of length, but it’s quite another matter to do it in 120”. If requirements allow a larger runout, the feature may be manufactured more readily with a .003” size tolerance and a special attribute of .012” total indicator runout tolerance.
Finish bored holes may be most readily quoted if specified completely for the required application. This list is a partial list of the attributes that may be assigned to a deep hole beyond the basics of size, position, and finish. Note that these attributes can be further defined with modifying symbols, tolerances and reference datums.
- Straightness
- Circularity or Roundness
- Cylindricity
- True Position
- Concentricity
- Circular Runout
- Total Indicator Runout
Selection of these depend largely on the form, fit, and function requirements of design for each part. For example, parts that rotate at high speed may require a low circular runout tolerance, but allow a wide straightness tolerance. The main bore may be solely for weight reduction and have no critical fit meaning a taper or other size variance is allowed, but all parts must be true and round for balance. Circular runout is better than total indicator runout in this example to allow size variation for economy.
Another part may be of a cylinder and piston application. For economy, various piston rings may be made to allow a large range of bore sizes, but function requires that each piece be of constant size and very straight. In this case a 4” bore with a 30” depth might have a .010” size tolerance with a cylindricity tolerance of .002”. Cylindricity offers composite control of circularity, straightness, and taper.
Other parts may require uniform wall thickness between OD and ID but allow a wide straightness tolerance. Such parts may hold pressure or transfer heat but be made from long tubing that is not straight. Apart from applying an attribute from the above list, such part drawings have a size and tolerance for the tube wall feature or a note to maintain a particular wall thickness.
Specifying only a part of the bore to have certain properties is a key way to reduce the overall cost of a deep-drilled part. Identifying these areas on the drawing can be done by designating a critical zone on the drawing or drawing notes. Selection of datum can also either improve accuracy, clarity, or reduce cost. Frequently the id of a deep part must be concentric to a long OD with a tight concentricity tolerance. If the whole OD is not critical, specify OD areas at the ends as datum and leave the balance of the OD with open tolerances. Sometimes bore concentricity matters only near the ends, save money by reflecting that on the drawing.
When applying concentricity as a bore attribute, consider that it does not control circularity. One can have a hole within size tolerance and concentric that is actually egg shaped. Circular runout is a composite of roundness and coaxiality. Total Indicator Runout is a composite control of circularity and coaxiality plus angularity, taper, and profile of a surface. For most deep-hole applications, circular runout or total indicator runout is the best way to define and encompass straightness and concentricity requirements of design. Also for deep holes, runout can be read directly in most cases with an indicator though not all shops have this capability.
We have seen that, although many choices exist for defining the form requirements of a deep bore, certain attributes can best apply to certain applications. It is the role of the design engineer to define the proper requirements. It is the role of manufacturing to confirm manufacturability and machine within supplied tolerances. It is the role of purchasing to convey requirements and communicate questions that arise regarding those requirements. In general, to maximize cost effectiveness, specify the roughest operations and widest tolerances. To maximize control of geometry for critical parts, specify tolerances sufficiently for all critical features. Be sure to contact the experts at American Hollow Boring Co. to review your specific project.
For further reading, we recommend you read part 4 of this series of articles on the topic of Deep Hole Geometry as Machined. Also refer to “Dimensioning and Tolerancing: ASME Y14.5M-1994 (Engineering Drawing and Related Documentation Practices)” by the American Society of Mechanical Engineers (ASME), 1995, ISBN-10: 0791822230.
