Saving time in determining tolerances

As you may know, fabricators embrace tolerances on drawings. The tolerance specification is regarded as something that is not to be questioned. When tolerances that are suitable for one trade are included on drawings for another trade—milling versus air-bending sheet metal, for example—something is questionable.

CAD templates and data entry forms can speed the process of making good drawings for manufacturing. Templates are just a starting point. To demonstrate the use of such templates, let’s walk through a process of prepping for a 2D drawing.

Shown in Figure 1a, the product is a grease gun. The drafting task is for the pivot link at the end of the pump handle.

To emphasize the fit requirement, Figure 1b isolates the pivot link (brown), the casting (yellow), and the pump handle (blue). The casting has machined features for connection to the pivot link. For tolerance planning, we expect that those machined features will repeat within ±0.004 in.

Connected to the other end of the pivot link, the blue pump handle is likely to be stamped from sheet metal with progressive tooling. Once the stamping line is tuned and running, its tooling will produce very consistent parts. Because of variation in paint and sheet metal thickness, we plan for the finished pump handles to repeat within ±0.008 in.

A pair of critical features for the pivot link are indicated in Figure 1c. The distance between the holes matters most when the pump handle is fully closed and the pump piston is (supposed to be) bottomed. If the link is too short (holes too close to each other), the pump action will not complete before the pump handle hits the cartridge tube. If the holes are too far apart, the pump handle will never seem to close enough. From 3D kinematic studies involving the grease gun model, we know that a hole-to-hole tolerance of ±0.014 in. will work for the pump link.

Note that the axle pins must pass through the pivot link to capture the casting or pump handle. Thus, the 90-degree bend angles are doubly important; axle pin fit and air gap work with mating parts. The distance between bends is, of course, important for the air gap as well.

Part of the preparation for making a 2D drawing is understanding how the part will be used. The goal is to avoid ridiculous tolerances that are wasteful. The 3D model reveals all.

Here’s a CAD tip: Use the Interference Detection tool. It can help you to verify that the CAD model matches the theory of design (Tools>Evaluate>Interference Detection). Figure 2 is a screen shot of the Interference Detection tool in operation. It shows two places where the pivot bracket is impossibly inside the casting.

While setting up for Figure 2, the author “ignored” 34 interferences. These are places where items screw or rivet together and are not related to the pivot link. The two remaining interference points are with the pivot link and the casting.

The Interference Detection tool reminds us that the casting is tapered—the secondary machining drills only the through-hole. Something in the design must change. For our product, we will make the pivot link wider (it was 0.516 in. and should be 0.518 in.) to clear the taper in the casting. Lateral slop in this linkage will not affect the function or utility of the pump.

Figure 3a is our first demonstration of a CAD template. In this example the template is a data entry form shown to the right in the figure. The form allows for drop-down selection lists—material, gauge, finish, among others. Such drop-downs reduce typing errors and speed the human’s data entry.

Figure 3b shows an example of a drop-down list for tolerances. In the sheet metal trade, the distance between holes is controlled by one process, laser cutting for example. The distance between bends and holes may be controlled by another process, a press brake for example. The convention of specifying hole-to-hole, hole-to-fold, and fold-to-fold tolerances for sheet metal is something suggested to me in the early 1980s by John Payne, at the time working for HP. (If you’re reading this, John, happy birthday!)

The Property Tab Builder Tool makes it easy to customize the drop-down lists to match your preference. In this example, the Property Tab Builder tool was used to create a property named “Tolerance.” Such a named property can save any value selected from a drop-down list. The form can be set up to allow (or deny) change to the selected value.

For our demonstration we selected “Hole-To-Hole ±0.006 Hole-To-Edge ±0.008 Fold-To-Fold ±0.014 Angles ±0.25°” as the default tolerance for this sheet metal pivot link.

Figure 3c shows the result of data saved in the 3D part as it appears on the 2D drawing. The red markup in the figure emphasizes information automatically displayed in the tolerance block on the drawing. This is our second use of a template, in this case a drawing template. The 2D drawing template uses a sheet format (a third template) that displays the value of a property named “Tolerance.”

The title block template includes the phrase “Unless Otherwise Noted.” By ANSI drafting standard, the default tolerance may be overruled by tolerances attached to individual dimensions.

Figure 3c is only an example. Had this been someone else’s set of templates, the tolerance property could be saved in the 2D drawing instead of in the 3D part. The advantage of saving the metadata—the “properties”—in the 3D part (or assembly) as opposed to the 2D drawing itself is convenience; the data entry form can be consulted while studying the assembly for selecting appropriate tolerances for components.

Returning to our example in Figure 3b, drop-down of tolerances might offer starting points for several trades—sheet metal fabricating, machining, sawing, and so forth. For example, a machined part might use “X.XXX ±0.006 X.XX ±0.012 X.X ±0.1 ANGLES ±0.25°.” In our example, our trade-agnostic 2D drawing template will display whatever the property “Tolerance” holds.

Figure 4 emphasizes a couple of places where the default tolerance has been overridden. The inside distance between bends cannot be less than 0.518 in. without interference with the casting. Thus, +0.014 in. and -0.000 in. are specifications suitable for general sheet metal fabrication.

As a side note, this sheet metal design could certainly be more difficult to fabricate with ±0.004 in. if the 0.518 changed to 0.522. That tight tolerance would limit the fabrication options—pretty much to stamping—and would make sense if rattle around the casting were an important consideration.

Gerald would love for you to send him your comments and questions. You are not alone, and the problems you face often are shared by others. Share the grief, and perhaps we will all share in the joy of finding answers. Please send your questions and comments to dand@thefabricator.com.