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

(continued from page 2)

Now It’s Time for BMX

You are now going to take the pattern you just created a step further. Some time ago I designed a blast box used in a methane-rich environment. Since the box contained electrical components, I needed an o-ring seal. The rule I used with this o-ring seal was the standard "space the bolt centerlines at a maximum of 10X the thread size."

During the conceptual design stages, the size of the box changed constantly. With each small change, I had to sit down and recalculate the bolt pattern. This really interfered with "designing-on-the-fly" when I wanted to make some quick changes to test a new idea. I was left wondering whether I could make the hole pattern "smart" enough to automatically adjust to the new size.

One way is to use a Datum Analysis feature to capture critical information and then include a few more pattern relations for brains. You will use PTC's Behavioral Modeling functionality to measure the two sides of the curve and hand that information to the pattern relations. This lets the pattern relation calculate the proper number of instances and spacing!

1. Create two Datum Analysis features that measure the two sides of the curve. To do this, click on the Datum Analysis icon or select from the Insert menu (Insert, Datum, Analysis).

2. Enter an Analysis Name—in this example, CURVE1 (Figure 5).

Figure 5

3. Click on the Next button. When you are prompted to select a curve to measure, select the side of the curve that the first point in the bolt pattern is on (Figure 6).

Figure 6		Figure 7

5. Repeat this process with the second section of the curve, making sure that you name this new analysis something like CURVE2. The model tree should look something like Figure 8. The two Datum Analysis features allow you to use the information about the length of the two sides of the curve in relations when creating the pattern.

Figure 8

6. Now you need to add a few parameters to fully and easily control the behavior of the hole pattern. You want to "parameterize" the offset from the edge of the plate as well as the distance of the corner holes from the edge of the plate. On the side menu, select Set Up, Parameters, Part, Create, Real Number. Call the first parameter HOLES_OFFSET and give it a value of 20. Create another one called CORNER_HOLE_OFFSET and give it a value of 50.

7. As you add more capability, you want to make sure the model is driven correctly. Make your curve offset equally from each side of the plate using feature relations, something like this:

sd31 = holes_offset
sd32 = holes_offset
sd33 = holes_offset
sd34 = holes_offset

While there are myriad ways to ensure this, the important issue is to make the model as concise and bombproof as possible.

Next: Redefining the Pattern >>>