New Partial Fillet and Chamfer Tool in SOLIDWORKS 2019

When working with complex geometry, one of the biggest challenges can arise when you need to add a fillet or chamfer to an edge and don’t want the fillet or chamfer to run along the entire edge, but instead only want the feature to exist along a subsection of the edge (see Figure 1).

Figure 1. The goal is to add a chamfer to this edge, but not to the entire edge.

As shown in Figure 1, the goal is to create a chamfer in the middle of the edge, but not to have this chamfer extend out beyond this central location. 

Prior to SOLIDWORKS 2019, you would need to perform a time-consuming work-around to achieve this.

Method 1Creating a Partial Chamfer Using a Cut Sweep

In pre-2019 versions of SOLIDWORKS, one approach would be to create a cut sweep feature along the desired section of the edge as shown in Figure 2.

Figure 2. The elements required to create a cut sweep feature along a subsection of an edge.

As you can see in Figure 2, creating a “partial chamfer” by generating a cut sweep would require several features. You would have to create a new 3D sketch representing the path of the cut sweep, a new plane at the end of this path, and a new 2D sketch representing the profile of the cut sweep (see Figure 3).

Figure 3. Attempting to generate a cut sweep of a partial chamfer – Sweep operation failed to complete.

Unfortunately, attempting to create this cut sweep would produce an error, indicating that the feature could not be created. This generally meant a lot of time would have to be spent troubleshooting the sweep path and profile to get the desired results. 

Method 2—Performing a Split Body Command

Another technique that was commonly used before SOLIDWORKS 2019 was the “Split-Chamfer-Combine” method that is shown in Figure 4. 

Figure 4. The elements required to perform a split, so that a partial chamfer can be created along this edge.

To prepare for the split command, you would create a 3D sketch along the section of the edge where you would like to add the chamfer. You would then create two new planes, one at each end point of this 3D sketch. You would then use these planes to perform a split body command, which would split the model into three separate solid bodies as can be seen in Figure 5.

Figure 5. The model has been split into three separate solid bodies.

Now that the model has been split into three separate solid bodies, a chamfer can be added (see Figure 6). 

Figure 6. The chamfer can be added to just one single body.

Since the model is split, the chamfer will only be applied to one of the bodies, as is shown in Figure 6. Before SOLIDWORKS 2019, once this chamfer was added, a user would finish up by combining these three bodies back into one single solid body (see Figure 7).

Figure 7. The model has been combined back into one single solid body.

After performing a combine command, the model is back to one single body, and there is now a partial edge chamfer.

Saving Time with SOLIDWORKS 2019

In the two examples above, you can see that while it was indeed possible to add a chamfer to only a subsection of an edge prior to SOLIDWORKS 2019, it also meant using some sort of work-around.  And these work-around generally required a lot of time, as well as some in-depth knowledge of SOLIDWORKS software and modeling techniques. In SOLIDWORKS 2019, these work-arounds are a thing of the past, and adding a chamfer (or fillet) to the partial edge of a model is as simple as click-drag-click.

Let’s start with the model in its original state—no sweep cuts, no splits, no chamfer (see Figure 8).

Figure 8. The model before adding the partial chamfer in SOLIDWORKS 2019.

Next, let’s begin the chamfer feature command.

Figure 9. Selecting the OFFSET FACE option for the chamfer.

After beginning the chamfer command, you must choose the option for OFFSET FACE. If you do not choose this option, you will not see the option for “Partial Edge Parameters.”

Figure 10. Choosing the option for “Partial Edge Parameters” and then dragging and dropping the start/end points.

After selecting the desired edge for the chamfer and choosing the chamfer type OFFSET FACE, you can select the option for “Partial Edge Parameters” as shown in Figure 10. You can then simply drag and drop the purple node to indicate where you would like the chamfer to begin. Last, you can drag the green node to indicate where you would like the chamfer to end.

Figure 11. The partial edge chamfer has successfully been created.

After pressing the green checkmark, you will see that your partial edge chamfer has been successfully created. 

Partial Fillet

By following these same steps, you can also create a partial edge fillet as shown in Figure 12.

Figure 12. Choosing the option for “Partial Edge Parameters” when creating a fillet.

The process for creating a partial edge fillet in SOLIDWORKS 2019 follows the same workflow as the process for creating a partial edge chamfer. You can simply begin the fillet command, then select the option for “Partial Edge Parameters.” After this is selected, you can drag and drop the purple and green nodes to indicate where you would like the fillet to begin and end (see Figure 13).

Figure 13. The partial edge fillet is completed successfully.


Creating a chamfer or fillet that runs along the subsection of an edge can be a frustrating and time-consuming challenge. Before 2019, SOLIDWORKS users had to come up with some type of work-around. Sometimes users created a cut-sweep to represent the partial chamfer or fillet. Other times users would split their solid body into multiple bodies, so that they could achieve the desired result.

SOLIDWORKS 2019 has added a terrific enhancement to the chamfer and fillet commands—enabling users to easily specify an edge they want to modify, and then drag and drop points to indicate where they would like their fillet or chamfer to begin and end along the selected edge. This capability will save users time and frustration, as well as allow them to get their products to the manufacturing and marketing teams faster than ever before!

About the Author

Toby Schnaars is a Certified SOLIDWORKS Expert from Philadelphia, Pa. He has been working with SOLIDWORKS software since 1998 and has been providing training, technical support, and tips and tricks since 2001.

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