Back in Doing the Splits: Part 1, we covered key details on basic splits. With Part 2, we saw the various keep and remove options and scenarios where we’d need to use them. Although we’ve made it most of the way through the options in the Split command, there are just a few left to investigate. In this last part on the Split tool, we’ll look at Extrapolation types, Intersection Elements and Half Space settings.
To Extend or Not To Extend: Extrapolation Type
By default, Extrapolation is on and set to “Tangency.” If a cutting element is too short to completely intersect the cut item, it’ll be extended. The extension is a straight line that is tangent to the point at the end of the curve. Most CATIA commands that extend items use this same approach.
If you’d prefer that cutting elements that are too short are not extended you can change this setting to “None.” Now, you’ll manually have to ensure that the cutting items are of adequate length.
Ignore No Intersecting Elements
In this scenario, there are six cylinders being cut by a yellow plane. All of the cylinders are separate features, so there are six items to cut and one cutting element. The results are as expected: All cylinders are cut at the plane, shown below.
This is great, until we start to modify the yellow cutting surface. Reducing the size of the surface until it no longer intersects all of the cylinders will yield an error.
If we anticipate that the cutting surface may continue to change and that it’s possible that we may need to cut all of the cylinders again, or even fewer of them, then it may be a good idea to enable “Ignore no intersecting elements.”
Now, as the yellow splitting surface is adjusted, any elements no longer being cut by the Split will simply be ignored, avoiding the warning messages. If we extend the cutting surface so that it again crosses on of those cylinders, then it’ll automatically be included.
Keep Elements in Half Space
First, the Keep Elements in Half Space option only applies if a plane is being used to cut items. A standard surface will not work here. Second, we’ll typically use this with non-connex elements – that is, elements that are a single feature, but have some distance between them.
A typical way to run into something non-connex is if you pattern a surface. The pattern itself is a single feature, but none of the items are directly connected and joined to each other. Another common way to get a result like this is to create a Join, but disable the “Check connexity” option.
In the image below, there is a pattern of cylinders, creating a non-connex feature. Planes are intersecting the second and fourth cylinders from the left. Our goal is to keep the surface area between the planes.
Creating a Split initially gives results like the image below: The cylinders beyond the planes are not cut, yet are still retained.
Checking “Keep Elements in Half Space” will only keep the surfaces in the “half” space between the Splitting items. The extra cylinders are removed.
A quick press of OK to finish the Split yields the final shape:
We’ve made our way through our various Split options, particularly as they relate to surfaces. Some techniques (such as selecting the side of the item that you’d like to keep) are essential to efficiently using the Split command. Some of the options are a bit more obscure, but are great to have when needed.
Keep in mind, you can also Split curves with other curves and in addition, you can also Split surfaces with curves or vice versa.
I hope you found some value in our Surface Split mini-series. If you’re looking for more information on general surfacing (including Splits), then the CATIA V5: Intro to Surface Design and Advanced Surface Design classes are excellent resources.
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