Machine to the Mean with CAMWorks

Oboe Wu | Comments | December 27, 2016

Have you ever defined asymmetrical tolerance requirements in your designs? Does this type of tolerances look familiar? A nominal width size of 110 mm with a tolerance range from+0.15 to -0.25 mm, or a nominal hole diameter of 85 mm with a unilateral tolerance window of -0.05 to -0.25 mm, requiring both limits on the smaller side of the nominal diameter.

I’d love to hear your thoughts in the comment area below. If you are a designer, where would you specify asymmetrical tolerances? If you are a machinist, how would you handle asymmetrical tolerances?

Prashant Kulkarni shared his experiences with GE Power and Water. Figure 1 shows a drawing that he encountered, in which a hole diameter was defined as 1.5 in with a tolerance range of +0.0035 to -0.005 in, along with other asymmetrical tolerance requirements.

image001Figure 1. A drawing with asymmetrical tolerance ranges. (Image courtesy of GE.)

The designers wanted to make sure that a 1.5-in drill is used, so the hole can’t be smaller than 1.5 in, except for the tolerance of the drill itself, which is 0.005 in.

On the other hand, for machinists, machining to the nominal dimension with an asymmetrical tolerance range would feel similar to driving a vehicle closely to one side of the lane but far away from the other side, rather than staying in the middle of the lane. The wiggle room on the nearside would be much smaller than the far side. One deviation on the near side could exceed the limit and scrap the part, while the same deviation could be tolerated on the far side.

You can manage to make it work if the upper and lower limits are spread apart on both sides of the nominal. It just increases the risks. However, for unilateral tolerances in which the limits are only on one side, machining to the nominal wouldn’t work at all because the nominal dimension itself is out of the tolerance range.

Therefore, a typical handling of an asymmetrical tolerance window is to calculate its mean dimension to reach a symmetrical tolerance range. In other words, machining to the mean, rather than the nominal, allows machinists to drive safely in the middle of the lane. The benefit is to even the penalization risks between the upper and lower limits, increase the finished part pass rate and save the overall manufacturing cost.

That was what the GE manufacturing engineers ended up doing to the drawing in Figure 1. They manually modified the model features to reach symmetrical tolerance ranges. For the example above, the hole size was tweaked to 1.515 ± 0.020 in.

But throughout a design, there can be a large number of asymmetrical tolerance ranges. This kind of manual modification can take lots of a manufacturing engineer’s time and introduce unnecessary human errors. To answer this challenge, CAMWorks came up with a solution shown in the green circle in Figure 2, “Machine to Mean.”

image002Figure 2. A “Machine to Mean” option in CAMWorks.

This option automatically assigns the cutter allowances to arrive at the mean sizes with symmetrical tolerance ranges, so that you don’t have to tweak the model manually or recalculate the tolerances any more.

Let’s take a look at one example as shown in Figure 3, in which the highlighted nominal pocket width size of 110 mm is defined with a tolerance range of +0.15 to -0.25 mm.

image003Figure 3. A nominal pocket width size is defined with an asymmetrical tolerance range, highlighted in green at the lower-left corner.

Don’s scratch your head yet. Instead of running the numbers in your head or on a piece of paper, you can now run the CAMWorks tolerance-based machine. Figure 4 shows that the milling contour operation is automatically created. Furthermore, please pay attention to the tree node where the mean tolerance value is calculated automatically as 0.025 mm in the green circle.

image004Figure 4. A contour milling operation is automatically created with a mean tolerance value of 0.025 mm.

If you double-click on this milling operation, you will see the highlighted side allowance 0.025 mm at the upper-left corner on the dialog box as shown in Figure 5.

image005Figure 5. The side allowance is automatically calculated as 0.025 mm.

By the way, the allowance stands for the amount of material to leave on the sides of the part for a later contour milling cycle. This value is the actual distance the cutter stays away from the finished part. The amount is defined per side. The allowance can be positive or negative. Negative values up to the radius of the tool can be specified and will cause the tool path to overcut the part.

Just in case you are wondering how the allowance is calculated, let me walk you through the steps. First, let’s calculate the mean width size, which is the average of the upper and lower limits, or (110.15 + 109.75)/2 = 109.95 mm. Then figure out the offset from the nominal size to the mean size—that is, 110 – 109.95 = 0.05 mm. Last, just evenly distribute the offset to both sides of the width feature, which is 0.025 mm as shown in Figures 4 and 5.

Here is another example as shown in Figure 6. The slot size is 30 mm wide and 70 mm long, with a unilateral tolerance zone on both the width and length from +0.1 to 0.0 mm.

image006Figure 6. A contour milling operation on multiple slots of a unilateral tolerance range from +0.1 to 0.0 mm.

Now you may wonder which nominal size to use here: the width of 30 mm or the length of 70 mm. The answer is that it doesn’t matter. What matters is the tolerance distribution. Let’s use the 30 mm as an example. The mean width is (30.1 + 30)/2, or 30.05 mm. Then the offset from the nominal size to the mean is 30 – 30.05, or -0.05 mm, so the cutter allowance on one side is half of that, or -0.025 mm, as shown in the tree node in Figure 6. You can verify it with the 70-mm length size yourself.

Please note the material allowance is negative here. It means that the cutter will overcut the part so that the openings are bigger than the nominal sizes, as required by the tolerance zones.

Now let’s capture the calculation in a formula as shown below, just in case you want to verify the allowances.

The material allowance = – (upper tolerance + lower tolerance)/4

However, the good news is that you don’t have to remember this formula, manually run these calculations or modify the tolerances any more. No matter how many asymmetrical tolerance ranges there are, CAMWorks takes the allowances into consideration automatically for the numerical control code programming. To learn more about machining to the mean size, please visit the CAMWorks product page.

About the Author


Oboe Wu is a SOLIDWORKS product manager with 20 years of experience in engineering and software. He is an advocate of model-based enterprise and smart manufacturing.

Recommended News