Join John Helfen for an in-depth discussion in this video Add intelligence to a rectangular pattern, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] We're now going to continue looking at that rectangular pattern tool, but what you can see on the screen is a modification to where we ended in the previous movie. What I did is I took the final result of the last movie, and I made a minor modification. What I did was I changed the overall length of this extrusion so that it's eight inches long. The reason for this is I wanted to show how we can build some intelligence into the model using parameters and some of the other settings in the rectangular pattern tool. To do this, we need to edit the rectangular pattern.
We can do that by double clicking on it in the browser. To bring back up the dialogue box that we created this pattern with in the first place. And we can look at a few of the settings. The ones that we really want to look at and that are most important, are really here at the bottom of each direction section. And that's the spacing. Spacing is set as the default. What that means is that there's going to be a distance of 1.25 inches between each occurrence here in this pattern. If we select the drop down again, we can check distance or curve length, and we're going to start with curve length.
I just want to show what it does, it's not something that's used very frequently, but I want to make sure you know it's there. What this does is takes the line you selected as the direction and uses that as its distance for the pattern. You can see here that it's grayed out the eight inches, and instead it's using the length of this line. The problem with this is this original feature is offset by a half inch. Therefore, the final instance of the pattern is also offset by a half inch. In this case, what we really want to look at is the distance option.
The distance is set to eight inches, and you can see the preview hasn't really updated, but we can manually enter seven and what that does is rather thatn set the distance to 1.25 inches between each occurrence is it says we want five instances within a seven inch pattern. Now, if we go ahead and select OK, it looks like the model's been updated, but we run into a problem if this core base feature changes again. If we were to return and double click on Sketch1 and set this to nine, and update the pattern you'll see that where essentially where we were before.
Rather than just setting the spacing, we changed it to distance, but we really didn't link it to the model in any way, so any change to the features before the pattern, has the potential to break the pattern. I'm going to go ahead and right click and select Undo to return our model back to where it was, the eight inches. And let's look at how we can add some intelligence here. What we can do is double click on the pattern again to edit it, and let's look at how we can add a parameter here that would help make this work more appropriately.
Instead of setting a curve length or spacing, we're going to leave it at distance, and what we're going to do is we're going to highlight all the text here, and we're going to click the arrow to the right side of that value. And we have a few options, we have the ability to measure something, and what we really want to look at is the Show Dimensions option. What it allows you to do is select a feature in the model, in this case the base feature. Left click on it and see all the dimensions that are driving that shape. The reason this is important is because we can highlight this seven value and left click on the eight value here on the model, and you'll see that it updates with d0.
This is the parameter name for this value. Now, what you can see is nothing's really changed here. We've set the spacing to distance, we've set this to a parameter that equals eight, and we see that the previews are updating, but what we can do is we can add a formula here. We can enter -1, which accounts for the half inch distance here, and the half inch distance here, but what's most important is that it will do this calculation based on whatever the value is for the width of the overall base feature.
This is important because if we select OK here, and then we return to the Sketch and double click on it, we can change this to, let's say, 10 inches, hit enter, it updates and when we finish this sketch it updates as well, and you can see that the holes are evenly distributed along this part. Let's go ahead and do that one more time. We'll double click the Sketch1. This time let's change it from 10 to five, and select the green check mark, and you can see the model updates. When we finish the sketch, all the holes still remain, they're just much closer together, and Inventor has automatically calculated what the distance between these are in order to meet the requirements that were set in that dialogue box.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers