SolidWorks Featured Author Blog: Fillet Techniques

Version 12

    https://files.solidworks.com/FeaturedFeed/faJuly.png

    Fillet Techniques

     

    From Machine design to Consumer Product design, creating Fillet features is something that you quite like do when creating your models. There are basically six types of fillets you can apply in SolidWorks: Constant, Variable, Full-Round, Fillet via Hold Line, Setback or vertex fillets and Curve Continuous Fillets. Let’s review them quickly.

     

     

    Constant Fillets – are the most basic and prolific type of fillet and are used in machine fabricated shapes to injection molded consumer product design. They can be easily applied on edges or faces with a single constant value or you can specify multiple constant values (value per edge or edge-set) per fillet feature.

    1.jpg

    Variable Fillets – have almost all the capabilities of Constant Fillets but with the addition that fillet values can be specified anywhere on the selected edges, which results in a transition of fillet value along the edge/s.  The user can apply as many values along the edge/s as they desire, although too many values results in a fillet that is difficult to make look smooth and manage.

    2.jpg

    Full-round Fillets – create a fillet between two opposing faces which share an adjacent face between them – i.e. thickness of a plate of steel; the side edge between the top and bottom face of the plate is “replaced” with a fillet which starts at the top face and ends at the bottom face, using the side face (removed face.) the fillet value is determined by calculating a tangent condition between all three faces. A Helpful way to quickly apply a full round is to click the Right mouse button immediately after selecting the 1st side face to advance the selection to the center face; then after center face selection, RMB again to move the selection to the 2nd side face.

    3.jpg

    Fillet by Hold Line –is a variable type of fillet (adjacent faces are used instead of edges as input) but its fillet values are controlled by model edge at the perimeter of the face/s being filleted. Hence, this is a fillet that accepts only faces as the selection.  It is a very powerful solution and especially attractive to the Industrial designer since it creates a very “stylized” solution.

    4.jpg

    Setback Fillet – is an option to the constant fillet. Vertex fillets cannot be created in of themselves but can augment the intersection of edges in which constant fillets are applied. It is called Setback because the user enters a value that is a distance from the vertex setback along the edge. This can result in a very nice solution by “rounding the corner with a transition between constant or multi-constant filleted edges.

    5.jpg


    A helpful cleanup tip is to use insert>Face>Delete>Delete w/fill and tangency to make the setback area a single smooth face.

    6.jpg

    Curve Continuous Fillets – in SolidWorks can be applied when using the face to face option. The Curve continuous (or C2) option applies a non-circular fillet solution based on an approximate fillet value. It is approximate, because the shape of the fillet is altered to conform to a curve continuous matching condition with the adjacent faces that it is applying the fillet between. Using this fillet type is essential on aerodynamic or consumer product design shapes when smoothness of transition is paramount.

    7.jpg

     

     

     

    Even with the arsenal of six different ways to apply fillets, there can still be times when Fillets are difficult to apply to your model.  There are a few common reasons why this might occur for your situation;

     

    1. Non-tangent intersection – The edges that you are specifying for the fillet are not tangent to one another, therefore the fillet stops and does not propagate along (default setting) the set of “seemingly” tangent edges. Sometimes fillets cannot find a geometry solution when the fillet stops at non-tangent intersection. In situations like these, sometimes you can apply your fillet solution by unchecking “Tangent propagation” and selecting each of the edges individually. In this way, the constant fillet solution is applied to each edge individually and therefore can sometimes find a total fillet solution.
    2. Self-intersection – in some cases when the designer is trying to apply a fillet to a set of continuous (tangent) edges, say the end face of a box which already has vertical fillets applied to it and when the fillet runs along the edge it encounters a rounded corner (existing vertical filleted edges) the fillet that is being applied is a larger value than the rounded edge that it needs to traverse. The SolidWorks Constant fillet can usually overcome this situation, but for anything other than a constant fillet (variable etc.) this situation will prevent the fillet from continuing around the edge. Good designers usually avoid this situation by the following rule-of-thumb: apply your largest fillets first to your design, and then apply progressively smaller fillets henceforth.  This results in good aesthetics since fillets on products naturally want to “flow” along edges and self-intersection and sharp resultant apexes are a thing to avoid aesthetically.
    3. Fillet Run-out – Most fillet problems are caused by what I like to term “unresolvable fillet run-out condition.” It is in situations like these where the fillet “runs off” the edge of the part and literally there is no geometric solution that can be attained.  There is a known solution to this problem which is known in the community as the “Atomic Bomb solution.” This technique, first invented by SW community icon Ed Eaton, applies a clever solution to this problem by simply temporarily eliminating the run-out problem before the fillet ever sees it. 8.jpg

     

    When it is suspected that there is a run-out issue, the technique calls for the designer to “chop away” the end of the fillet edge (at the end vertices)  by either extruding a cut over it or applying a split line around the vertex and deleting the resultant split-line face, turning the solid body into a surface body. At this point the fillet can be applied. Once applied a Fill Feature is applied to fill the hole at the end of the fillet and turn it back to a solid Body. The following example illustrates this solution:

     

     

    1st. Create a simple sketch to Split-Curve the area in question9.png

    2nd. Insert>Face>Delete>Delete and remove the faces within the split.  The solid body is now a single surface body.

    10.png

    3rd. Insert the fillets on the two edges. Adjust the split sketch accordingly to fit the value of the fillet so as the fillets never touch each other at the open boundary.

    11.png

    4th. Now use the Insert>Surface>Fill command.  Click on one of the edges of the open boundary and the RMB and choose “Open Loop”. This will automatically gather up all the edges of the boundary saving you time.

    12.png

    5th. In the Fill Command Property Pane, check “Apply to all edges” and then select “Tangent” from the dropdown selection box above it. Also check “Merge Result” and “Try to form solid.” Click Okay.

    13.png

    6th. Turn on View>Display>Tangent edges removed to see your result.

    14.png

     

    There you have it. this technique usually solves those tricky filleting problems by creating a custom blend solution and resulting in an aesthetic and functional result.

     

    Look to SolidWorks providing additional fillet functionality in the future. In fact a new fillet feature is being introduced and tested in Beta right now. If you have not already done so, please go check it out by signing up for SolidWorks 2014 Beta here.

     

    ***

     

    A degreed Industrial Designer, Mark has worked in the product design industry for over 25 years for such companies as Atari, Hewlett Packard and IDEO. Joining SW in 2004 as a Product Manager, he currently is Senior Product Manager for Definition.

     

    Note:
    - You can view all of the Featured Author Blogs by visiting our Index.
    - Subscription Services required for full access.
    - Looking for more learning resources? Visit the SolidWorks Resource Center.