Creating Hole Patterns Around the Edge of a Plate-The Smart Way

Almost anyone designing with Pro/ENGINEER® has encountered the problem of placing a bolt-hole pattern around the edge of a plate. The first time I had to do this, I just sketched the thru-holes I needed. When I had to use that same plate in an assembly, though, I almost broke my wrist assembling all the washers, bolts and nuts to those holes! Even with the "repeat" functionality it was pretty tedious.

Then I realized that you could pattern all those washers, nuts and bolts in the assembly if there was a reference pattern to attach them to. But I thought the only way to have a pattern was to create one for each of the four sides of the plate. This made things a bit easier and somewhat eased my wrist complaints. Anyone who has tried patterns, however, knows that their use is not straightforward. In the interest of speed, I used identical patterns. The problem is that one hole often falls off the plate and then the entire pattern fails. With general patterns, a hole falling off the edge doesn't cause as many problems, but the bolt assembled to that "floating" hole just doesn't compute.

I have encountered this four-part pattern approach many times, in many different companies. For quite a while, I thought there was no better way. I even tried table-driven patterns, but the headache of calculating each hole location every time the plate changed was nastier than the wrist-ache from creating four patterns and placing the four sets of bolts, nuts and washers.

Then I discovered relation-driven patterns. Using relations, Pro/ENGINEER can control the distance between patterned holes (or whatever dimensions for whatever features) without making you calculate the coordinates for each individual instance. One pattern, no calculations to place every hole, and you can make it stay on the plate so the bolts don’t float.

Creating the Pattern

The basic idea is to attach the holes to a curve that is offset from the edge of the plate. Not only is the pattern safe from "falling off" the plate, but it is one-dimensional (following the curve) rather than two-dimensional. This means you can concentrate on the hole spacing without having to deal with XY coordinates.

1. Create a plate 1000mm x 500mm x 20mm.

2. Sketch a curve offset 20mm from the edge of the plate so that it looks like Figure 1.

Figure 1

3. Now create a point on this curve (Datum Point, On Curve, Actual Len).

4. Pick anywhere on the curve. When Pro/ENGINEER asks for the length on the curve where you want your point, enter 30. You will now carefully attach all your following features to that point.

5. I prefer to use the "hole" feature, so create a datum axis for the hole centerline using Datum Axis, Pnt Norm Pln or Pnt On Surf (for curved surfaces).

6. Select the top surface and the datum point that you recently created. Add a coaxial hole and reference the just-created axis.

7. Put the point, axis and hole in a group. Your model and model tree should look like Figures 2 and 3.

Figure 2		Figure 3

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