our digital manufacturing ecosystem
Global Manufacturing Network
People on the ground
3D Printing Materials
Urethane Casting Materials
Digital Manufacturing Resources
Learn about fictiv
2021 State of Manufacturing Report
DFM for CNC Machining
Tolerance Stack Ups 501: Going Beyond Mechanical Fit and Into Predictive Design
Thank you for subscribing!
Fabricating a product without deviations from the original design is extremely complicated. Even if you are able to get an instance comparable to your design intention, it is nearly impossible to always achieve the same exact dimensions in a batch process. That being said, you can decide how much a fabricated product can deviate from the original intention in order to be accepted. In manufacturing, this range of acceptance is defined by limits which are called tolerance limits. These tolerances represent the variations between nominal dimensions (original intention of the design) and the maximum and minimum values of a dimension that still guarantee a fitting design; or in simple words: a controlled margin of error.
Let’s say you specify a round solid bar of 100mm length with Ø50mm that will fit inside of a hole of another component. You place an order to fabricate 200 of these Ø50mm rounds bars and when you receive them, you realize not all of them measure Ø50mm, but you get values like Ø53mm, Ø47mm, Ø51mm, Ø49mm, with a lot of variation. The bars also vary in length and when you take a closer look, you realize they are not perfectly circular. Can you still use them? If not, can you reject them and ask the vendor to redo at no cost? How close to the Ø50mm should you really be?
There is an international standard that not only helps you to answer these questions but guides you to minimize inconsistencies while keeping manufacturing cost in consideration. The best part is that, since it was created by an international committee, it allows you to be on the same page as companies all around the world so there are no misunderstandings. That standard is ISO 2768.
To explain the content of this standard and its parts, we will be using a real engineering example. Figure 1 shows a vehicle engine with a compressor for AC. The component that supports the compressor and connects it to the engine is our focus; we’ll call it the “compressor base”. We will start with a prototype that is made from an aluminum casting, then machined and drilled.
Once a 3D model is defined with nominal dimensions, we proceed to identify which features need tight tolerances and which ones are allowed to deviate more so we can communicate these requirements on the fabrication drawing. The reason for differentiating levels of tolerance requirement is simple: if all dimensions require tight tolerances, then the cost of the part will increase significantly due to more demanding tooling/fixtures, operator skills and scrap/rework requirements (learn more about how tolerance drives manufacturing effort). Delivery time will also be increased since each part of the batch would need a strict quality check to corroborate each dimension, and as shown in this example, some components have complex compound geometries that are not easy to quantify.
When you design a part, it is important to ask yourself what is the main function of each feature. Some dimensions could be critical since their purpose is to align to other parts, therefore the margin of error should be controlled. On the other hand, there are features with dimensions and locations that are not as critical so they can have more flexibility during fabrication. As you would expect, it is a tradeoff between accuracy and cost.
For our compressor base example, Figure 2 shows which features should actually have a tight tolerance and which ones are permitted to vary more. Keep in mind the illustrated classification is meant to serve as an example, so it can differ from other designs. It is your responsibility to develop a proper classification based on your product’s function. In our case, the drilled holes to connect to the Engine’s block and to the Compressor need to be aligned and positioned correctly, therefore their tolerance is in the fine category (see #1 and #2 on Figure 2). The contact surfaces between components are also important for alignment (#3 and #4), but for this particular example we were able to use a medium tolerance since a more accurate machine roughness than the one we were getting from the vendor did not benefit alignment enough to justify the extra cost. On the other hand, the purpose of the ribs is to add strength, thus their wall thickness can be defined with an acceptable minimum value with a less rigorous tolerance as long as it meets the lower limit (#5, coarse tolerance). The main body of the base was defined as very coarse tolerance (#6) and finally we define references planes or datums to control the rest of the dimensions (#7, fine tolerance since we will be dimensioning from these surfaces). Keep in mind that for other designs, features like ribs, fillets and chamfers might be critical, depending on their function.
ISO 2768 is divided into two parts, and both help to simplify drawings by defining precision levels as general rules:
A drawing could be specified as ISO2768-mK for example, which means, as general rule, it should meet the tolerances ranges for “medium” seen on Part 1 and tolerance class “K” seen on Part 2. By including the ISO2768 specification, you are simplifying your drawing avoiding writing tolerances for every dimension and feature. We mentioned general rule because you might have exceptions when a dimension needs tighter tolerance than the ones of ISO2768. This is normal and common, so always keep an eye on the drawing title block for general tolerance requirements and be informed if there is any special part specification or project requirement.
You should also be aware that there are several other standards that work with similar dimensional concepts. You probably have heard about GD&T which is related to ISO 2768 Part 2. Learn more about the basics of GD&T here.
Table 1 shows the precision levels or tolerance class designation for linear dimensions. One application is the dimension between holes for our compressor base example (see Figure 3).
Table 1: Tolerance Classes – Linear Dimensions
In a similar way, Table 2 shows the tolerances for external radii and chamfers.
Table 2: Tolerance Classes – External Radii and Chamfers
And to complete Part 1 of ISO 2768, we have Table 3 which defines the tolerances for angular dimensions. Notice the tolerances units on Table 3 are degrees and minutes as expected for an angular dimension. In Part 2 we will be defining a new concept called “perpendicularity” whose units are actually length (mm) despite the fact that it controls two surfaces in angle.
Table 3: Tolerance classes – Angular Dimensions
Part 2 defines three tolerance ranges H, K and L. These are different from the fitting and clearance tolerance grades that also use letters and numbers.
Similar to Part 1, we have nominal ranges and deviations, but the difference is how we define those deviations. An example is shown in Figure 4: instead of defining an upper limit and a lower limit, we define a region between two references (i.e. parallel planes), so the fabricated surface should lie in that region. This may sound more complicated, but it actually makes sense when you measure a part and realize that if you place a caliper to measure two rough surfaces, you get different measurement values due to the roughness of the surfaces. We define datums to use as reference for dimension and controlling how much deviation is acceptable. As illustrated on Figure 2, we picked three perpendicular planes for the base compressor (datum A, B, C on Figure 1).
Table 4 defines Flatness and Straightness tolerance classes. A surface might have an excessive roughness. In our compressor base, the contact surfaces between compressor and base and the contact surfaces between base and engine are important, so their flatness will be specified in the drawing.
Straightness controls how much a surface varies within a specified line on that surface. Another use of straightness is for the axis of a part to control how much bend or twist is allowed.
Table 4: Straightness and Flatness Tolerances
As mentioned before, Perpendicularity has distance units (mm or in). Similar than Flatness, we define two planes separated by a gap equal to the permissible deviation on Table 5. We control the 90 degrees angle indirectly, since we are measuring if the surface is in the permissible region (see Figure 6)
Table 5: Perpendicularity Tolerances
Table 6 shows the tolerances for Symmetry – permissible deviations for two features on a part that are uniform across a datum plane.
Table 6: Symmetry Tolerances
And the last table of Part 2 corresponds to Run-out, which is the total variation that a surface can have when the part is rotated around a datum’s axis. Notice that the marked surface is on tolerance despite the fact that it is not perfectly cylindrical.
Table 7: Run-out Tolerances
You may have noticed that there is no table defined for parallelism. This is because ISO2768 Part 2 defines parallelism as equal to the numerical value of the size tolerance or the flatness/straightness tolerance, whichever is greater. Both of these tolerances are covered earlier in the article.
ISO 2768 covered some of the tolerance and geometric characteristics used in industry and this is a great place to start. However, there are more standards and they expand in the concept of Geometric Dimensioning and Tolerancing (GD&T), whose symbols are shown in Table 8. We recommend you read more about GD&T and ASME Y14 next.
Several companies have been implementing a method called Model Based Definition (MBD) whose goal is to increase collaboration by including all GD&T, tolerances and datum information in 3D models rather than 2D drawings. In theory, this is possible since some CAD software have tools to include these symbols and values as parametric information. I believe that replacing 2D drawings with 3D models as the record of authority would have to be implemented carefully, but who knows? Engineering is constantly evolving.
Table 8: GD&T Terms
Download the calculator
Download the worksheet