How Machining Allowance Affects Accuracy in CNC Operations

As the quality requirements for mechanical processing products continue to improve, considerable time and effort have been devoted to exploring methods and measures to enhance product quality. However, the impact of machining allowance on product quality has often been overlooked. Many believe that having a margin during processing minimizes its effect on product quality. In practice, it has been observed that the size of the machining allowance for parts directly influences the overall quality of the product.

 

If the machining allowance is too small, it becomes challenging to eliminate residual shape and position errors, as well as surface defects from the previous processing steps. Conversely, if the allowance is too large, it not only increases the workload for mechanical processing but also leads to higher consumption of materials, tools, and energy. More seriously, the heat generated from removing a large amount of machining allowance can cause parts to deform, complicating the processing and negatively affecting product quality. Therefore, it is crucial to maintain strict control over the machining allowance of parts.

 

1 Concept of machining allowance

The machining allowance refers to the thickness of the metal layer that is removed from the machining surface during the machining process. This allowance can be categorized into two types: process machining allowance and total machining allowance.

The process machining allowance is the thickness of the metal layer cut from a specific surface during a particular machining process. This measurement depends on the difference between the dimensions before and after adjacent machining processes. In contrast, the total machining allowance is the combined thickness of the metal layer removed from a specific surface throughout the entire machining process, from the raw material to the finished product. Essentially, it is the difference between the size of the blank and the final part size on the same surface. The total machining allowance is calculated as the sum of the machining allowances from each individual process.

It is important to note that errors can arise during the manufacturing of the blank as well as throughout each machining process. Consequently, both the total machining allowance and the process machining allowance are variable values, which means that minimum and maximum machining allowances can occur.

 

In the accompanying diagram, the minimum machining allowance is defined as the difference between the minimum process size of the previous operation and the maximum process size of the current operation. On the other hand, the maximum machining allowance is the difference between the maximum process size of the previous operation and the minimum process size of the current operation.

The variation range of the process machining allowance, which is the difference between the maximum and minimum machining allowances, is equal to the sum of the dimensional tolerances for both the previous and current processes. Typically, the tolerance zone for the process dimensions is specified in the direction in which the part enters the body. For shaft components, the basic size corresponds to the maximum process size, while for holes, it pertains to the minimum process size.

2 Analysis of the influence of machining allowance on machining accuracy

2.1 The influence of excessive machining allowance on machining accuracy

During the machining process, parts inevitably generate heat due to cutting. This cutting heat is dissipated in several ways: some is carried away by iron chips and cutting fluid, some is transferred to the tool, and the remainder is transferred to the workpiece, leading to an increase in its temperature. The temperature rise is closely related to the size of the machining allowance. When the machining allowance is large, the rough machining time will be extended, and the cutting volume will increase, resulting in more cutting heat and a further increase in workpiece temperature.

One significant consequence of raised temperatures is the potential for deformation of the part, particularly for materials that are sensitive to temperature changes, such as stainless steel. This thermal deformation is an ongoing issue throughout the machining process, which complicates machining and negatively impacts product quality.

For example, when machining slender shaft parts like screw rods, the one-clamp-one-top machining method limits the degree of freedom in the length direction. If the workpiece temperature rises too high, thermal expansion occurs. When this extension in the length direction is constrained, the workpiece can bend and deform due to stress, creating challenges for subsequent processing. The bending deformation of the workpiece post-heating can be illustrated in a diagram.

If machining continues under these conditions, the protruding areas may be processed until the final product is achieved. However, once the part cools to room temperature, it can deform in the opposite direction due to stress, leading to shape and positional errors that affect quality. A diagram can illustrate the bending deformation of the workpiece at room temperature. Additionally, when the diameter expands, any enlarged parts will be removed, resulting in cylindrical and size errors after cooling. When grinding precision screws, thermal deformation can also induce pitch errors.

 

2.2 The influence of too small machining allowance on machining accuracy

The machining allowance for parts should be neither too large nor too small. If the allowance is too small, residual geometric tolerances and surface defects from the previous process may not be eliminated, ultimately affecting product quality. To ensure the machining quality of the parts, the minimum machining allowance left in each process must meet the basic requirements of the minimum allowance for the previous process.

The schematic diagram illustrating the components of the minimum machining allowance for the inner hole of a specific part is shown in Figure 4. In Figure 4a, the part to be machined features an inner hole. If the axis O1-O1 of the hole deviates from the reference axis O-O during the previous process, a position error (n) will occur. Additionally, the inner hole may exhibit a cylindrical error (p), such as taper or ellipse, as well as a surface roughness error (h), as depicted in Figure 4b. To eliminate these geometric tolerances before boring, the single-sided minimum machining allowance for the boring process must account for all these errors and defects.

Moreover, it is essential to consider the inevitable installation errors of the workpiece during the boring process. This includes the error (e) between the original hole axis O-O and the rotation axis O’-O’ after the workpiece is installed, as shown in Figure 4c. Along with the dimensional tolerance (T) for the boring process, the minimum machining allowance (z) for this procedure can be expressed with the following formula:

z ≥ T/2 + h + p + n + e (single-sided allowance).

Figure 4 Diagram of the components of the minimum machining allowance

The errors in different parts and processes can vary in both their values and manifestations. Therefore, the machining allowance should be determined based on specific treatments for each process. For instance, a slender shaft is prone to bending and deformation, which can result in a generatrix straight line error exceeding the diameter size tolerance range. In such cases, the machining allowance should be increased appropriately for processes that utilize tools, such as floating cutters, which help position the machining surface itself. In these instances, the impact of installation error can be neglected, allowing for a reduction in the machining allowance. Conversely, for finishing processes primarily aimed at decreasing surface roughness, the size of the machining allowance is chiefly dependent on the desired surface roughness.

 

3 Reasonable selection of machining allowance

3.1 Principles for machining allowance of parts

The selection of machining allowance for parts is closely linked to several factors, including the material, size, accuracy level, and processing methods employed. It should be determined based on the specific context of each part. When deciding on the machining allowance, the following principles should be observed:

- Use the minimum machining allowance necessary to reduce processing time and costs.

- Leave adequate machining allowance, particularly for the final process, to ensure that the required accuracy and surface roughness specified in the drawing are achieved.

- Consider the deformation that may occur during the heat treatment of the parts, as neglecting this can lead to scrapping the components.

- Take into account the processing methods and equipment, as well as any potential deformation during machining, when determining the allowance.

- Factor in the size of the prototype parts being processed; larger parts typically require larger machining allowances due to the increased likelihood of deformation from cutting forces and internal stresses.

By adhering to these principles, you can ensure an effective and efficient machining process.

 

3.2 Methods for Determining Machining Allowance

3.2.1 Empirical estimation method

The empirical estimation method is frequently used in production practices to determine machining allowances. This approach relies on the design experience of process personnel or comparisons with similar parts. For instance, the machining allowances for components such as the rudder stock, rudder pin, intermediate shaft, and stern shaft in a ship under construction are established based on the years of design experience of the personnel involved.

Given the significance of the workpieces and the influence of factors like the large volume and high stress of the forging blanks, specific allowances are left during machining. After rough turning the outer circle, a 6 mm semi-finishing allowance is applied. Following semi-finishing turning, a 3 mm finishing allowance is used, and finally, a 1 mm grinding allowance is designated for finishing.

To avoid waste caused by insufficient machining allowance, the empirical estimation method often results in larger machining allowances than necessary. This method is particularly suited for single-piece or small-batch production.

 

3.2.2 Table lookup correction method

The table lookup correction method involves creating a table that compiles data and information on machining allowances gathered from production practices and experimental research. This table is then revised to account for actual machining conditions in order to determine the appropriate machining allowance. This method is widely utilized in the industry. The machining allowances for the outer circumference of bearing parts after rough aluminum turning and grinding are presented in Table 1 and Table 2, respectively.

 

3.2.3 Analytical calculation method

The analytical calculation method is used to determine the machining allowance by thoroughly analyzing and calculating various factors that influence it, based on test data and formulas. This method provides an accurate and cost-effective machining allowance, but it requires a substantial amount of comprehensive data. However, it is not as straightforward and intuitive as the other two methods, which is why it is currently used less frequently.

 

4 Conclusion

In actual production, the methods for manufacturing various part blanks may be subject to change. For example, the production of centrifugally cast stainless steel sleeves may switch to using rolled and welded steel plates. Similarly, components such as the cooler end cover, motor base, and gearbox, which were initially sand-cast, may now be produced as welded parts. These changes introduce many uncertainties into the production process, making it challenging to predict shape errors for these parts. As a result, the three methods discussed in this article for determining machining allowances are not suitable for these applications. Instead, they should be adapted based on the specific circumstances encountered during production.

Table 1 Machining allowance of the outer circle of shaft parts after rough turning and fine turning mm

Table 2 Machining allowance for grinding the outer circle of shaft parts mm

 

 

If you want to know more or inquiry, please feel free to contact info@anebon.com

Anebon offers new fashion designs for China CNC Machining Service and Custom die casting service. The company utilizes various foreign trade platforms such as Alibaba, Globalsources, Global Market, and Made-in-China.