Surfacing Approach to Import Modifications - Part 1

Have you ever imported a part that still needed some work to be done on it, and you weren’t sure where to begin? Did the geometry fail import diagnostics and now you’re stuck with a collection of surfaces? This excerpt will cover some surfacing tools that may help you get out of the mud with your part with a few import modifications.

For this example, it is possible to do this same modification using solid tools. The purpose of this tech tip is to demo some surfacing tools instead. Knowing these tools becomes very important when working with imported geometry that isn’t a solid, or that has faulty faces.

Import Modifications Method 1: Convert to Surfaces

We start this method by choosing what portions of the geometry we need to reuse. In this case, we need a sketch that depicts the edges of the solid body. We do this by using the Convert Entities tool, . A tip for this is to click the “Collect all inner loops” (new in SOLIDWORKS 2016) in the property manager. This will grab the edges of the pockets. This will allow us to quickly get a sketch of all the edges we need to extend.

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Using the Extrude-Surface tool, ,I can create a wall that is 20mm deep, which will compensate for the overall thickness that this part needs to be when it’s finished.

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Next, I need to copy the original flat face of the part and move that up to the edges of my new surface walls. I’ll do that with the Offset-Surface command,, and offset a surface for my new top face of the part.

Now I have a bunch of surfaces representing the extended portion of the model, and a solid body that was the original import. I want everything to become one solid body of the current shape on the screen.

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I don’t want to combine the surface bodies to the solid body, but instead I’m going to turn the solid into surfaces by deleting the original top face, as it will not be needed. You can do this with the Delete-Face tool,.

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Now I can select all of my surface bodies and use the Knit Surface tool,,to combine them, and choose “Create Solid” to turn this part back into a solid. The “Merge Entities” check box will allow you to remove model edges of surfaces that were new within the same face, or to remove an edge between faces with the same underlying geometry. Keep in mind that if your surfaces do not form an enclosed watertight region, the “Create Solid” option will be grayed out.

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Merge Entities Cleared

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Merge Entities Checked

That was a quick introduction into surfacing tools that can be used to manipulate geometry. I like to consider this the “manual” method as it is a few steps, and requires a higher level of design intent to get to the finished product. Check out the video Tech-Tip of this blog on our YouTube channel.

There are other tools in SOLIDWORKS that can make this same chore quite a bit easier! Check back for Part 2 where I discuss and demo two more methods to tackle this modification.