There are times when the SolidWorks default chamfer tool is unable to perform the tasks users have in mind, creating an error message that the chamfer could not be built due to geometry conditions. In these cases, users have to take into their own hands to accomplish these tasks instead. An example would be the following, creating a chamfer on a cylinder with a slanted edge as shown in the image above.
As shown from the figure above, creating a chamfer on the edge may seem trivial at first, but upon closer inspection, the angle between the two faces actually vary along the edge, whereby the angle near the top is acute, while at the bottom it is obtuse. This obtuse angle at the bottom contradicts the chamfer feature as it is already, in a sense, chamfered. Solidworks have a hard time propagating the chamfered edge and shows the user an error. However, as CAD users, we do not give up and look for an alternate solution. Here I have come up with one out of many possible solutions, to address this solution.
1. Firstly we create a duplicate of the slanted surface using the offset surface tool.
2. Set the offset to be zero. This will create a duplicate face that will eventually replace the existing face.
3. Hide the duplicated surface so that the original surface can be viewed.
4. Use the delete face tool to delete the top face. This action will also cause the original solid body to be converted into a surface body. Select the delete option in the delete face property manager.
5. After deleting the face, we would like to remove part of the surface body that will be replaced with the chamfer surfaces. Create a sketch line on the plane perpendicular to the slanted edge. Set the distance of the line to the size of the chamfer, and add a parallel relation to the slanted edge.
6. Using the trim surface tool, select the sketch line created as the trim tool, and select the top part of the surface to be removed.
7. After deleting the face, we are ready to create the chamfer surface. Select the ruled surface tool. For the surface type, we will choose tapered to vector. This option will allow us to create a surface along an edge at an angle. The angle will be based on the vector determined by the user. For the reference vector, select the top of the duplicated surface done in step 2 and set the angle to 45 degree. Set the distance to any value as long as it exceeds the duplicated surface so that we can trim and stitch them together later.
For the edge selection, choose the slanted edges of the cylinder body. You may need to change the direction of the vector if the surface is going in the opposite direction from the second image shown below.
8. Using the trim surface tool again, we will use the mutual trim type to remove the excess surfaces generated from the previous operations. Select the two surfaces generated previously in the surfaces box. Then, select remove selection option and select the excess surfaces in the remove selections box. We now have all the surfaces needed.
9. In the final step, use the knit surface tool and select all the surfaces. Check the create solid option to convert the surfaces back into a solid. We now have the part completed with the proper design intent.
Hopefully this post has provided some insight on how to leverage the surfacing tools in Solidworks in situations where the default tools are unable to create the desired design.