Adding Associative Dimensions to Hole Notes

Posted September 22, 2008

by Community Admin1

Include Bolt Circle Diameters in Hole Notes!

Machines are made up of many parts that vary from simple to complex. And these parts are fastened together in many ways. The most common ways are with screws, bolts or rivets. In order to use these fastening methods, holes need to be located in the mating parts. These holes need to be lined up with a reasonable amount of accuracy for ease of assembly and proper fitment.

Many times, on circular parts or parts with circular features, holes are arrayed in circular patterns. Holes laid out in this fashion are very easy to machine with modern machining processes. When it comes to documenting these circular patterns there are many schools of thought. One method is to dimension the diameter of the bolt circle or pitch circle. Another method is to add the bolt circle diameter to the hole callout.

One of the important features of Autodesk® Inventor® is the ability of the dimensions to update as their associated features change. Along the same lines, it is possible to link values included in Notes with their associated features. This makes it relatively easy to add associative bolt circle diameters to hole notes, ensuring that the circular hole patterns line up between components when it is time for assembly.

The Setup

Imagine that you are working on the design of a large aluminum duct. This duct will be made of cast aluminum, and will transition from a rectangular opening to a circular opening. The two ends of the duct are located perpendicular to each other.

The duct is completely designed at this point, with the exception of the hole pattern in the circular end. The hole pattern consists of eight 13.5 mm holes arrayed in a circular pattern, sharing a center with the circular flange where the holes are located.

Once this hole pattern has been added, you need to document it in the drawing. Like the part itself, the drawing is complete with the exception of the holes located in the circular end. Adding the bolt circle diameter to the hole note is relatively easy. The problem is, you would like the hole note bolt circle diameter to update accordingly if the hole pattern in the part changes.

Let’s look at how this is accomplished.

1. Begin by creating a sketch on the flange face. Project the outer edge of the flange so we can reference the center in the future.

2. The next step is to sketch a line from the projected center straight upwards to somewhere on the flange.

3. Select the point at the top end of the line and change it to a Hole Center by selecting the Hole Center type  from the standard toolbar.

4. Next, create a linear dimension from the hole center to the center of the flange. Just accept the current dimension value for now. Exit the sketch.

5. In the parameters dialog, create a new parameter and give it a value equal to your bolt circle diameter. In this case, a value of 290mm will suffice. Be sure to check the parameter for export.

6. Locate the parameter of the dimension we created earlier. Make it equal to the bolt circle diameter parameter divided by two. This will adjust the previously created hole center to the correct distance from center.

7. Next, we will create a hole through the flange. In this instance, use a diameter of 13.5mm.

8. Once the hole is created, create a pattern of holes on the plate. Reference the outer edge of the flange for the Rotation Axis. Enter a quantity of eight.

9. Next, you can open or switch to the drawing. The views of the duct will update to reflect the new holes. Add center marks  to properly document the pattern.

10. This just leaves the small counterbores on the lower face of the flange. To remove these, we will use the Delete Face tool. With the Heal option on, select all of the faces associated with the counterbores.

11. Edit the hole note and add the quantity using the add quantity  tool. In this case, the quantity was added before the hole note.

12. Now for the cool part. Edit the hole note text and add the bolt circle diameter by linking to the parameter from the model. Follow the steps below to achieve this. Select the component; set the source to User Parameters; choose the correct parameter by name; set the precision; and insert the linked value.

13. All that is left is to add BCD after the value to denote Bolt Circle Diameter.

The Conclusion

Using this workflow, it is very easy to add associative values to your hole notes. If circular bolt patterns are something your organization deals with frequently, a standard hole note can be created. This standard hole note would simply require you to populate the linked value after placing the note.

Leveraging this technique, associative values can be added to any text object within a drawing. This procedure makes it very easy for you and your designers to maintain associative notes that adhere to your organization’s standards. You will experience a reduction in the chance of errors, allowing you and your team to spend more of your time creating, rather than checking.

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