An Advanced Breakdown: More Features of the SOLIDWORKS Fillet Tool
The Fillet command on the Features toolbar.
In Part 1 of our two-part series on the SOLIDWORKS Fillet command, we reviewed the details of the Constant Size Fillet tool. In today’s article, we will review the remaining three types of fillet features: the Variable Size Fillet, the Face Fillet and the Full Round Fillet tools.
The four types of fillets available in the Fillet feature.
The previous article discussed some options in the Fillet command that appear in all four types of fillets, including the options for tangent propagation and preview type shown in Figure 1.
Figure 1. The common options that appear in all four fillet types.
This article will discuss the unique options and settings that appear in the other fillet types. We will begin with the Variable Size Fillet feature.
The Variable Size Fillet
The Variable Size Fillet is an extremely valuable tool in SOLIDWORKS. By adjusting the properties of a variable size fillet, we can create a fillet feature which blends from a smaller-radius fillet to a larger-radius fillet, similar to Figure 2.
Figure 2. An example of a part with a variable size fillet applied to the upper edges.
After beginning a fillet command from the Features toolbar, the Variable Size Fillet tool may be initiated by selecting the second icon in the Fillet property manager.
Figure 3. The property manager for the Variable Size Fillet tool.
The property manager for the Variable Size Fillet (shown in Figure 3 above) looks very similar to the property manager for the Constant Size Fillet tool. The sections discussing setback parameters and fillet options were covered in the previous article, so we will not be reviewing them today. Instead, we will be focusing on the section on the Variable Radius Parameters menu as shown in Figure 4.
Figure 4. An overview of the Variable Radius Parameters section of the Variable Size Fillet property manager.
Fillet Method and Profile Type
When examining the property manager options listed under Variable Radius Parameters, the first option listed will be a choice of fillet method, which can be either a symmetric or asymmetric radius as shown in Figure 5. This option essentially controls whether the fillet will be generated with a circular or elliptical profile when examined at a cross-section.
Figure 5. A comparison of working with a symmetric fillet method (left) and an asymmetric fillet method (right).
As we can see in Figure 4, the Fillet Method option may be toggled to generate a circular or elliptical profile, depending on the desired results for our model. The option for fillet profile type, found a little lower in the Variable Radius Parameters menu, gives us similar options to control the radius profile.
The Variable Radius Parameters option allows us to set a profile type for the fillet feature.
There are four options available for profile type: Circular, Conic Rho, Conic Radius and Curvature Continuous. The Circular option will generate a profile with a circular cross-section. This could be considered a “standard” fillet. The Conic Rho (or Conic Radius) option will yield an asymmetric conic fillet profile, which is a two-dimensional curve whose shape can be obtained by taking the intersection of a plane and a cone. The Curvature Continuous option will yield a profile which will show as a spline when examined in a cross-section. The spline’s curvature will begin and end with precisely the same curvature as its adjacent faces and will gradually blend to the curvature found at the peak of the fillet.
Figure 6. The Variable Radius Parameters section allowing us to choose a profile type for the fillet feature.
As we can see in Figure 6 above, the options for profile type will give us some additional capabilities to achieve the desired geometry for models. When working with the Continuous Curvature option, we can generate an almost-indistinguishable transition between the fillet and its adjacent faces. This is especially important in the field of consumer product design, where it’s all about putting the best face forward with smooth transitions and no hard edges. This smooth transition can be viewed by changing the display style to zebra stripes, as shown in Figure 6. Note that the radius value is really more of a distance value for setback, since the radius in these profiles is no longer circular in nature.
Attached Radii and Control Points
The next section of the Variable Radius Parameters menu allows us to choose which edges will be filleted. After selecting an edge, SOLIDWORKS will automatically generate control points along the selected edge as shown in Figure 7.
Figure 7. Control points are automatically added to the selected edge.
These control points will allow us to set the varying radius values along the edge. The number of control points may be adjusted within the property manager. In Figure 7, there are three control points evenly spaced along the selected edge. We can adjust the location of the control points by left-clicking and dragging one of the control points. We can also create additional control points by holding CTRL and then left-clicking and dragging a control point. We can remove control points by single-clicking a control point and pressing the Delete key.
To assign a radius value to a control point, left-click on the control point. A callout will appear in the graphics area indicating that a radius has not yet been assigned to this control point. Type in the desired radius value at each control point.
Figure 8. A variable radius with a radius value assigned to all control points.
In Figure 8, we can see that a variable radius fillet has been created with the radius at one end starting with a value of 0.125 in. At the control point located 25 percent of the way along the edge, the radius remains at 0.125 in but then increases to 0.5 in at the control point which is 50 percent of the way along the edge. It remains at 0.5 in until we get to the control point which is 75 percent of the way along the edge. From here, it transitions to the final end point of the edge and increases to a radius of 1.0 in.
If there are any control points which have not yet been defined, they may all be set simultaneously by entering a value into the radius section of the property manager and then choosing the button labeled Set Unassigned. Similarly, we may change every single control point to use the same radius by setting a value and then choosing the button for Set All.
Smooth Transition vs. Straight Transition
The transition from control point to control point is automatically calculated by the software to yield a smooth transition. The option for a smooth transition or a straight transition as shown in Figure 8 is primarily an option to control the transition from the start and end points of an edge to an adjacent face. Consider the following example part in Figure 9. Our goal is to create a new variable radius fillet on the middle section.
Figure 9. A model to which we are going to add a variable size fillet in the middle section.
When working with a variable size fillet, it is common to transition from an existing filleted face. In the example in Figure 9, we have a fillet on either side of the edge to which we are going to add a variable size fillet. Depending on whether we choose a straight transition or a smooth transition, we will get the following results.
Figure 10. The results of using the option for a smooth transition (top) and straight transition (bottom).
As we can see in Figure 10, the smooth transition will create a variable size fillet that begins and ends with a smoother blend between existing filleted faces. The straight transition will begin the transition at its control point with a radius assigned, without regard for the surrounding faces. In a situation similar to Figure 10, the smooth transition would likely be the desired option. However, there are cases where the straight transition offers results more in line with what we are looking for.
The Variable Size Fillet is an amazingly powerful tool. By creating control points and assigning radius values, we can easily create smooth transitions from a larger radius to a smaller radius along a single edge, or a continuous series of multiple edges. If we want to generate a more exotic shape, we can experiment with the options available in the Fillet Method and the Profile menus.
Now that we have examined the options available in the Variable Size Fillet tool, let’s take a look at the Face Fillet tool.
The Face Fillet
The Face Fillet tool is often referred to as “the sledgehammer” of the available fillet commands. Although it requires a bit more set-up, this feature will often succeed in rebuilding and generating desired geometry where other fillet types have failed. After beginning a Fillet command from the Features toolbar, the Face Fillet tool may be initiated by selecting the third icon in the Fillet property manager as shown in Figure 11.
Figure 11. The Face Fillet icon.
This tool is so powerful because it can overcome geometric inconsistencies in and around the filleted region. When we examine the model in Figure 12, we see that there are a number of small sliver edges and faces in the corner area of the model.
Figure 12. A model with sliver edges and small faces.
This model demonstrates a situation where adding curved faces and drafted features has created a very busy area in the corner of the model. These small faces and edges will make it quite difficult to apply a constant size fillet or a variable size fillet to this region. However, the Face Fillet option should be a good solution here.
When examining the Face Fillet property manager, we are prompted to choose two sets of faces. One set of faces goes in the upper box and the other set of faces goes in the lower box. Wherever these two groups of faces intersect, a new fillet will be generated. This could be one single intersecting edge or it could be multiple intersecting edges (if multiple faces are added to either box). The great thing about the Face Fillet tool is that these faces don’t have to intersect when the tool is applied. SOLIDWORKS will generate a virtual edge at a hypothetical intersection and the Face Fillet feature will use this virtual edge as a basis.
In the example shown in Figure 12, we would add the following faces to the the Face Fillet property manager:
Figure 13. A face fillet is created by selecting two faces and generating a virtual intersecting edge.
Figure 13 shows that the face fillet has no problem with this type of scenario. It requires a bit more set-up since we need to select the faces rather than the edge, but this extra work is well worth it because it can help you generate an otherwise unsolvable fillet.
Face Fillet-specific Options and Tools
The Face Fillet tool utilizes a number of settings and options we reviewed earlier when discussing the Variable Size Fillet tool. Fillet Method, Profile and Overflow options are all available in the Face Fillet command. The Face Fillet tool does, however, have two unique and powerful settings. These settings, Chord Width and Hold Line, are found in the Fillet Method pull-down menu.
The Chord Width option in the Fillet command is a great tool as it allows us to specify a chord distance, rather than a radius, to define the fillet shape. In situations where you have complex angles coming together, this tool will be a great time saver.
In Figure 14, we can see that a parallelogram has been cut into the model with a 30-degree draft angle. In the four corners of this cut we have added a Constant Size Fillet feature.
Figure 14. An example of using a constant size fillet in the four corners but getting results that do not appear uniform.
Figure 14 shows an example of using a constant size fillet, but the results do not appear uniform even though they all use the same radius value of 0.25 in. In this common scenario, we have two acute angles and two obtuse angles, which combine with the cut’s draft angle to create a compound angle in each of the corners. The traditional solution would be to experiment with the radius value in each of the pairs of corners until the desired result was achieved and the four corners looked uniform. This would often be done simply with trial and error, a process which is very time-consuming.
Using the Face Fillet option, we can choose to assign a chord width to each of these four corners.
Figure 15. Using the Chord Width option, we can get a reliable and uniform result from all four corners.
As shown in Figure 15, we can create four separate Face Fillet commands. In each of these four features, we can set the chord width to the same value, which would result in a much more uniform and consistent result in each of the pocket’s four corners.
The other option which is unique to the Face Fillet command is the Hold Line option. This great tool allows users to create a split line to use as a guide for the Fillet command. Let’s consider the following example, where we have created a constant size fillet with a radius of 0.50 in:
Figure 16. An example of getting unexpected results from a Constant Size Fillet
In Figure 16, we can see that the constant size fillet looks good on the straight edges, but it yields some unexpected results once it gets to the curved faces at the top and the bottom of the slope. In a situation like this, we could create a split line on the model and use this split line as a hold line.
To create the split line, we will start by creating a new plane, offset from the sloped face by 0.5 in.
Offsetting a plane from the sloped face by 0.5 in.
Next, we can begin the Split Line command from the Features toolbar. We will choose the Intersection option and choose the plane and the outside faces of the part.
Creating a split line.
The result from following these steps is that we now have a new set of edges created where the plane intersects the four outer faces of the model.
The model now has four new edges created from the split line.
Next, we can begin a Face Fillet feature. To do this, add the lower sloped face to the box for “Face Set 1” and add the four upper outer faces to the box for “Face Set 2” as shown in Figure 17. Then, set the Profile option to Hold Line and select one of the split line edges (we only need to select one).
Figure 17. A Face Fillet feature being created with the Hold Line option.
As we see in Figure 17, the face fillet being created no longer asks for a radius value. Its geometry and radius are now being driven by the location of the split line that we created and selected as a hold line.
Figure 18. A completed Face Fillet feature using the Hold Line option.
When we compare the results in Figure 18 to those in Figure 16, we see that using the Face Fillet feature with the Hold Line option for creating a fillet across complex geometry will yield more consistent and reliable results by automatically generating a variable radius value which is dependent on the location of the Hold Line.
Whenever you find yourself in a situation where the constant size fillet or variable size fillet are not yielding the desired results, the Face Fillet tool should be considered. It offers some great tools that are not found in other fillet types, including Chord Width and Hole Line.
Now that we have reviewed the Face Fillet feature, let’s have a look at the final fillet type, the Full Round Fillet tool.
The Full Round Fillet
The Full Round Fillet tool is the fourth and final button on the Fillet property manager. This fillet is a unique command that does not have a radius value input. Instead, we are asked to select faces from the model to populate three boxes: “Face Set1,” “Center Face Set” and “Face Set2” as illustrated in Figure 19. The only other options for the full round fillet are for tangent propagation and previews, both of which we have already covered.
Figure 19. The Full Round Fillet property manager.
When creating a full round fillet, SOLIDWORKS will completely remove the “Center Face Set” and replace this selection with a filleted face which is tangent to “Face Set1” and “Face Set2.” For example, Figure 20 shows a model with a rib in one of the corners. This rib is angled and has draft applied on each side.
Figure 20. A model with a rib in the corner.
We could use a constant size radius to apply a rounded face to the top of this rib, but we would have to measure the width at the top of the rib and create two fillets. This would leave us with an undesired edge in the middle of the rib. These fillets would also need to have their dimensions changed if the rib’s width were changed, so a far more elegant solution would be to use the Full Round Fillet tool.
Figure 21. Selecting the faces for a full round fillet.
As we can see in Figure 21, we can use the Full Round Fillet feature to select the three different face sets. Once complete, Figure 22 shows us that the “Center Face Set” will be eliminated and replaced with a nice curved surface tangent to “Face Set1” and “Face Set2.”
Figure 22. A completed full round fillet.
The Full Round Fillet feature can be a great time saver when working with features such as a rib, which commonly need to be rounded off along the exposed face. Another application of the Full Round Fillet feature is to round off the entire exposed edge of an enclosure. The feature is not limited to a single face, so multiple faces may be selected in each face set box to get the desired results.
Figure 23. A complex variable radius generated using the Full Round Fillet feature.
Figure 23 shows an example of a model with variable wall thicknesses and several complex curves. This is a great example of how powerful the Full Round Fillet feature is. We can generate the fillet shown in blue by simply selecting three faces; one inside face of the model for “Face Set1,” the upper exposed edge face for “Center Face Set” and one outside face as “Face Set2.” Once we select these three faces (and have “Tangent propagation” selected) SOLIDWORKS will generate a complex variable radius fillet running around the entire upper exposed face of the container.
In Part 1, we covered the first and most common type of fillet: the Constant Size Fillet feature. Today we dove a little deeper into some of the more advanced filleting tools available in SOLIDWORKS. Each of these tools has its own unique sets of options and settings that will help you achieve the desired results for your models so that you (and your customers) will be happy with the nice, smooth geometry.
About the Author
Tobias Richard is a SOLIDWORKS elite applications engineer 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.