Creating Partial Fillet on an Edge
By: Chevy Kok
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Figure 1: Sample Image of a Partial Fillet Along an Edge.
Have you ever wondered how you can create a partial fillet on your SolidWorks models, like the one shown in Figure 1 above? Currently, if you use the fillet feature, the fillet will propagate along the edge. Even if you split the edge into two, the fillet will also propagate along the entire edge. (Refer to Figure 2). We will discuss how we can approach this issue by utilizing Library Features in SolidWorks.
- Figure 2: Current Options in Fillet Available in SolidWorks Fillet Feature.
To create a library feature, we will need to create a extruded-cut feature. Let’s start by creating the fillet arc by using a 3-point arc. Add tangent relations to the arc and the straight edge. Ensure also that the end points of the arc are coincident to the edges of the model.
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Finger 3: Create Radius of Fillet Using 3-Point Arc.
Complete the sketch by closing it up. Add dimensions to the arc and make it a link value. Link the dimensions of the arc to control the size of the other sketch entities.
- Figure 4: Close Sketch and Link Dimension Values
With the sketch created, perform an extruded-cut feature and key in any random value for Blind Depth. You may wish to rename the dimension name of this.
- Figure 5: Extruded-Cut Feature. Key in any value for blind depth.
Now that we have created the feature to represent the partial fillet, let’s save this into the design library. Please bear in mind that the face on which we started the sketch, the edges which we used to add relations to and the dimensions added will be used to position our library feature. To add the newly created cut feature into the Design Library, just click and drag the feature and drop it into the Design Library Task Pane. You will be prompted to save this file as a library feature (*.sldlfp).
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Figure 6: Creating Library Feature. Drag and Drop Feature into Design Library
Let’s open the file (*.sldlfp) we have just created and see it’s contents! Upon examining the Feature Manager, there are an extra few folders in this file; References and Dimensions. References are defined by the plane this feature is sketched on and edges where relations are added to the current feature sketch. The Dimensions folder contain the dimensions we have added to the sketch. Inside the Dimensions folder, we have ‘Locating Dimensions’ and ‘Internal Dimensions’. Locating Dimensions will be dimensions used to position the feature when inserted into the part. Let’s drag and drop the dimensions representing the radius of the arc and the depth of cut into the Locating Dimension folder.
- Figure 7: Feature Manager of Library Feature. Assign Locating Dimensions.
Let’s see how we can use this newly created library feature to create our partial fillet. With a model opened, drag and drop the library feature onto a planar face (this will be the sketch plane of the cut feature). You will be prompted to select edges to locate the feature.
- Figure 8: Inserting Library Feature and Positioning Feature.
After adding the cut feature, you can control the dimensions of the fillet radius and depth of cut by changing the Locating Dimensions in the Property Manager. Once you are happy with the preview, click OK and you are done! With this library feature created, you can add partial fillets effortlessly!
- Figure 9: Changing Dimensions of Partial Fillet
Chevy Kok is the Technical Development Manager at SeaCAD Technologies Pte Ltd (www.seacadtech.com) in Singapore. He is a member of the technical crew at SeaCAD Technologies who distributes, supports and conducts training of SolidWorks in Singapore and in the Philippines.
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