Thursday, 6 November 2014
Generating tapped holes on non-planar (cylindrical) faces.
As a SOLIDWORKS Elite Applications Engineer, I like to keep my eye on the SOLIDWORKS Forum so that I can pass on advice when questions are asked. Occasionally, I’ll find a question that has been asked that is best answered with a step by step guide rather than a one line answer.
One such case is a question that was posed recently by a SOLIDWORKS forum member who asked “how to make a threaded hole using holewizard on non-planar surface (cylindrical surface)?”
There are a few replies on similar questions on the SOLIDWORKS Forum which indicates that this user is not the only user with this question. Below is the process that I have used many times for adding hole wizard holes onto cylindrical faces that hopefully you may find useful.
This example is based on a cylindrical tube that I would like to add a tapped hole to.
I find that the easiest starting point is to generate a reference plane for positioning the hole, as often the standard planes are not suitable for positioning.
Step 1: To generate the positioning plane (Insert > Reference Geometry > Plane), select the cylindrical face so that the plane is tangential to the face. Then select another piece of geometry (in this case the Top Plane) so that you can choose the angle of the new reference plane.
Step 2: Once the plane is in place, select start the Hole Wizard tool (Insert > Features> Hole > Wizard), and select the type of hole that you would like. Then click on the Positions tab. At this stage, you can now select the new reference plane to generate a 2D sketch. But for this example, I have chosen the 3D Sketch button to demonstrate how to use this option. When using this option, SOLIDWORKS allows you to sketch directly onto the cylindrical face and will dynamically preview the hole location before you click to place the hole.
Step 3: Whilst adding locations for the Hole Wizard, SOLIDWORKS used standard sketch tools. Once you have clicked to place a hole, you can then switch between the sketch tools in the Command Manager Sketch tab. To allow me to add the required relations and dimensions to the 3D sketch that will locate the hole, I first added a construction line that was Coincident with the centre of the hole, and also with the circular end edge of the cylindrical face.
To define the geometry, I then added in an On Plane relation between the between both ends of the line and the plane that was created in step 1. Finally, I added a dimension to the line to specify the distance of the hole centre from the end of the cylinder.
One of the main reasons that I use this method for applying Hole Wizard Holes to cylindrical faces is that it gives me the best editing capability. Due to the creation of the reference plane tangential to the cylindrical face, if the diameter of the cylindrical face changes, the plane and all associated geometry will update automatically. As well as this, the angle of the reference plane can be changed to modify the angle of the threaded hole. Also, the hole position along the cylinder is controlled by a single dimension from the end of the cylinder.