ONE-DIMENSIONAL TOLERANCE ANALYSIS AND TOLERANCE STACKUP

Audio: One-dimensional tolerance analysis and tolerance stackup – part 1

In my previous article, Engineering tolerances – Introduction, we discussed the plus/minus tolerances, how to specify them on the drawing and what general tolerances are. In this article, we will talk about the basics of the one-dimensional tolerance analysis and tolerance stackup and how to convert tolerances. We will show you two methods that we can use for the tolerance stackup analysis: Worst-case tolerance analysis and Statistical tolerance analysis.

In this article, we will not consider Geometrical Product Specification (ASME standard name: Geometric dimensioning and tolerancing – GD&T). Instead, this topic will be addressed separately.

Introduction

The easiest way to define tolerances is to add them randomly to the drawing because we know how to do it in our CAD software, send it to our manufacturer, and hope that our parts will fit. But, on the other hand, there is also an expensive way; we call our supplier and ask the tightest tolerances they can achieve and then define them on the drawing. But this would cost us an arm and a leg to manufacture.

The proper way of defining the tolerances is to understand which dimensions are functional and which are not, how our dimensioning technic is adding up to the accumulation of the tolerances, which of our individual tolerances are influencing the most our accumulated tolerances, which of the tolerances we can make larger and which of them we must make tighter. This approach will give us the best ratio between quality and price.

The quality of our products is always imperative, and we are always trying to achieve the highest product quality. However, suppose we cannot deliver the product to our customers at a reasonable price. In that case, even the best product will die on the market because we could not get our manufacturing price under control.

This effect is visible when you have more than one part in your product. For example, imagine that you have 50 different parts 2 – 5 % more expensive only because of over-defined tolerances on your drawings. Then you specified unnecessary surface finishes on these parts, coatings, etc. Further down the line, you have an assembly process that you have not adequately defined and 5 min longer assembly time, etc. In the end, you end up with the overly expensive product that your competitors are selling for half of the price and the same level of quality.

With this approach, you would end up out of business pretty soon. Always have your customers in mind and put yourself in their shoes. You also would not pay for the same product double price if you have the alternative to buy it less expensive for the same level of quality.

In the context of price, as a mechanical design engineer, you can influence the overall cost and the quality of the product, starting with a single component. You can choose different materials, different manufacturing processes, different surface finishes, different tolerances, etc. This article will focus on tolerances and how to analyze one-dimensional tolerances to achieve the optimal quality and manufacturing price.

Tolerance analysis

The first step of the tolerance analysis is to clearly understand the tolerances defined on the drawing and prepare them in the format usable in tolerance stackup analysis. The second step is performing stackup analysis. The term tolerance analysis encompasses both these steps.

In the first step, we will analyze all of the tolerances defined on the drawing and understand the mutual connection between different dimensions and tolerances. For example, if we have an assembly, we will investigate the assembly procedure and the relationship between the different parts. After correctly understanding the various connections between the parts, we will select the distance (gap or interference) we want to analyze.

The next thing that we will do is prepare the tolerances in the format that is usable in tolerance stackup analysis, converting all of the tolerances into equal bilateral tolerancing (if you are not familiar with the terminology, check Engineering tolerances – Introduction).

Tolerance stackup

The tolerance stackup is a tool that allows us to understand the cumulative effect of multiple tolerances. Usually, we analyze the distance or clearance between the features (or parts) that are not dimensioned. The result of the tolerance stackup represents a nominal clearance or interference. With the use of the tolerance stackup, we are getting the numerical answer for the questions like:

Will the shaft fit into the bearing?
Will the pin fit within the hole?
If we assemble these components on top of each other, will there be interference with the housing?
Can we fit two plates in the groove?
What is the worst-case biggest length of the plate? etc.

With the results obtained from the tolerance stackup, we can determine if a change must be made on the part (or assembly) geometry, dimensions, and/or tolerances. We can also use the stackup analysis to optimize the tolerances on our drawing and save manufacturing costs.

Tolerance analysis working steps

Defining the distance to calculate

Let us investigate the example of the simple shaft drawing (simplified for the sake of the lesson). We have five different dimensions defined with different tolerances.

We can easily calculate for five dimensioned features expected manufacturing dimensions. However, we are interested in calculating the manufacturable nominal value and the tolerance of non-dimensioned features.

Now when we know what distance we want to calculate, we will mark one end with the letter “A” and the other end with the letter “B.”

Tolerance conversion

Before we start converting different tolerances into equal bilateral tolerancing for more straightforward navigation through the dimensions, we will define the number to each one of them.

We can see that we have a few different types of tolerances defined on the drawing. Previously we said that in order to perform the stackup analysis, we need to convert all tolerances to equal bilateral tolerances.

If you are unfamiliar with the terminology, check Engineering tolerances – Introduction.

Conversion of the negative unilateral tolerance to equal bilateral tolerance

Dimension number one is defined as negative unilateral tolerance. The first thing that we need to do is to calculate the upper (ULS) and lower (LLS) limit of size:

ULS = 37.2 + 0 = 37.2

LLS = 37.2 – 0.5 = 36.7

The next step is to determine the tolerance value:

T = 37.2 – 36.7 = 0.5

And our equal-bilateral tolerance value is:

T/2 = 0.5 / 2 = 0.25 – ± 0.25

The last step is to adjust the nominal value of the dimension:

N = LLS + T/2 = 36.7 + 0.25 = 36.95

In this case, our adjusted equal bilateral tolerance is 36.95 ± 0.25 mm.

General tolerances

Dimension number two has no visible defined tolerance, but that does not mean there is no defined tolerance value. Usually, the standard for general tolerances is defined in the title block of the drawing (for more information about the title block, check Basic elements of engineering drawings). Most often, it is stated as ISO 2768 – mK (for more details, check Engineering tolerances – Introduction). Please do not make this mistake and forget about the general tolerances!

If we look up in the ISO 2768 tolerance table:

Equal bilateral tolerance for dimension number two is: 10 ± 0.2 mm.

Conversion of the unequal bilateral tolerance to equal bilateral tolerance

Dimension number three is defined as unequal bilateral tolerance. The first thing that we need to do is to calculate the upper (ULS) and lower (LLS) limit of size:

ULS = 100 + 1 = 101

LLS = 100 – 2 = 98

The next step is to determine the tolerance value:

T = 101 – 98 = 3

And our equal-bilateral tolerance value is:

T/2 = 3 / 2 = 1.5 – ± 1.5

The last step is to adjust the nominal value of the dimension:

N = LLS + T/2 = 98 + 1.5 = 99.5

In this case, our adjusted equal bilateral tolerance is 99.5 ± 1.5 mm.

Conversion of limit dimensions to equal bilateral tolerance

Dimension number four is defined as the limit dimension. In this case, the upper (ULS) and lower (LLS) limits of size are already calculated:

ULS = 11

LLS = 9

The next step is to determine the tolerance value:

T = 11 – 9 = 2

And our equal-bilateral tolerance value is:

T/2 = 2 / 2 = 1 – ± 1

The last step is to adjust the nominal value of the dimension:

N = LLS + T/2 = 9 + 1 = 10

In this case, our adjusted equal bilateral tolerance is 10 ± 1 mm.

Conversion of the positive unilateral tolerance to equal bilateral tolerance

Dimension number five is defined as positive unilateral tolerance. The first thing that we need to do is to calculate the upper (ULS) and lower (LLS) limit of size:

ULS = 23.2 + 1 = 24.2

LLS = 23.2 – 0 = 23.2

The next step is to determine the tolerance value:

T = 24.2 – 23.2 = 1

And our equal-bilateral tolerance value is:

T/2 = 1 / 2 = 0.5 – ± 0.5

The last step is to adjust the nominal value of the dimension:

N = LLS + T/2 = 23.2 + 0.5 = 23.7

In this case, our adjusted equal bilateral tolerance is 23.7 ± 0.5 mm.

The drawing of the shaft with the adjusted equal bilateral tolerances would look like this:

Typically we would not change the defined tolerances on the drawing into the equal bilateral tolerances. This is only done to make the stackup analysis easier. Dimensions and tolerances on the drawing will stay the same, and you will adjust them based on the tolerance stackup results.

Determining a positive or a negative dimension direction

The last step before we can move to the tolerance stackup is to define a positive or a negative dimension direction. This step is essential because it will help us determine which dimensions need to be added together and which ones need to be subtracted to get the correct value of the missing gap or interference.

As we already stated, we are interested in the missing distance A-B. To define the dimension direction, we will define the origin of each dimension in a counterclockwise direction starting from point A and finishing at point B. Each dimension’s origin is at the end of the previous dimension.

Dimension number 1 will have its origin in point “A.”

Dimension number 2 will have its origin at the end of dimension 1, etc.

The next step is to define the positive and the negative direction. The positive direction will be in the direction from point A to point B.

The final step is to define which dimension is in a positive direction and which one is in a negative direction. If the arrow on the dimension is pointing in the direction “A-B” then the dimension is marked with the “+” sign. If the arrow on the dimension is pointing in the opposite direction than the “A-B” direction that the dimension is marked with the “-” sign.

After the tolerance analysis on the drawing is done and the directions are defined, we are ready to move on to the tolerance stackup analysis.

Worst-case tolerance stackup analysis

The worst-case tolerance stackup analysis is used to determine the gap variation or interference, assuming that all dimensions will be manufactured at their maximum or minimum limit (upper or lower limit of size).

In the table below, we will write the values of the dimensions with the positive and the negative values together with the corresponding tolerances. The nominal distance value equals the sum of the positive direction dimensions subtracted from the sum of the negative direction dimension. Tolerance, however, is the sum of all tolerances.

The missing distance dimension is 18.85 ± 3.45 mm.

Statistical tolerance stackup analysis

The statistical tolerance stackup analysis is used to determine the gap variation or interference with the assumption that not all dimensions will be manufactured at their maximum or minimum limit. The dimensions will likely approximate the normal distribution. Most of the dimensions will be closer to their nominal value than either extreme.

We will use RSS (Root-Sum-Square) method. When tolerances are calculated with the RSS method, in 99.7% of cases, the manufactured tolerances will be inside this range. Generally, the statistically calculated tolerances will have smaller values than tolerances calculated with the worst-case tolerance stackup.

In case we want to have a slightly more conservative approach, the RSS can be multiplied by the adjustment factor. We will use the adjustment factor of 1.5.

RSS tolerance can be calculated with the following formula:

Where: T_n represents tolerances in the stackup analysis.

In plain words, the RSS tolerance is equal to the square root of the sum of all squared tolerances in stackup analysis. Let us look into the previous example:

The starting point for the statistical tolerance stackup analysis is the same as for the worst-case tolerance stackup. The only difference is that we additionally need to calculate the squared tolerances for each dimension, add them and calculate the RSS tolerance.

The missing distance dimension is 18.85 ± 3.06.

Comparison between the worst-case and statistical tolerance stackup analysis

Our stackup analysis showed us that for:

worst-case stackup, the missing distance dimension is 18.85 ± 3.45 mm.

statistical stackup, the missing distance dimension is 18.85 ± 3.06 mm.

We can see that the statistical stackup calculated tolerance is lower than the worst-case stackup calculated tolerance, even with the adjusting factor. But what this means to us?

This means that we can actually “loosen” up tolerances on some dimensions. For example, if we would change dimension number three from 99.5 ± 1.5 mm to 99.5 ± 1.8 mm, we would get the RSS tolerance ± 3.4. This means that in the 99.7% manufacturing dimension of the missing distance will be 18.85 ± 3.4 mm. From this point of view, we would get almost the exact manufactured dimensions as we previously had with the worst-case stackup, but we would have looser tolerances in this case. Looser tolerances mean that your supplier has a larger room for error, which results in a lower manufacturing price.

I would suggest that in your calculations, you use both methods. This will only add a few additional fields to your calculation sheet, but it will give you better insight into the overall tolerances.

Closing words

Now you have an excellent overview of one-dimensional tolerance analysis and tolerance stackup. In the One-dimensional tolerance analysis and tolerance stackup – part 2, you can read more about the influence of the dimensioning technics on tolerance stackup and how to create the tolerance stackup report form.

However, I suggest you go through the text once more and identify areas you think need more understanding and clarity. Then, once you have identified those areas, start building up your knowledge in those areas.

To make it easier for you to find related posts, check the “Further reading” chapter below. Do you have any questions or need something to be clarified better? Leave a comment below, and I will give my best to adjust the post accordingly.

Do you like what you read? Then, share it with your friends, colleagues, and on your social media channels. And if you want to become a part of the Newtonians, make sure to subscribe to our newsletter!