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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.

Resetting the SOLIDWORKS registry

Over time within SOLIDWORKS it is possible to make a wide array of customisations to your user settings and also your user interface. It can be hard to keep track of these changes if you are editing them on a daily basis like I do. Also, we all know that system updates have been known to damage registry files that SOLIDWORKS needs to be able to function correctly.

So if you would like to fully reset all of your SOLIDWORKS preferences, or if you have noticed strange behaviour or missing icons since a recent Windows update. One option to resolve your issues it to reset the registry entry for SOLIDWORKS.

Firstly, be very careful when making modifications to the registry as this may cause serious instability on your system. As such, you will need full administrative permissions on your computer to be able to edit them.

The following guide illustrates how to create a fresh copy of the SOLIDWORKS registry for the current user of the machine in a Windows environment. This registry includes the system options and customisations that a particular user has set up. Examples of the types of elements that this controls are file locations, custom toolbars and system options. By creating a fresh copy of this registry, you will revert SOLIDWORKS for the current user back to default settings as if SOLIDWORKS is a new installation.

This process will not work correctly if SOLIDWORKS is currently running, so the first step is to save all relevant work and exit SOLIDWORKS.

The registry is controlled by your operating system and in Windows the process for   accessing the registry is as follows;
 

Click on the Start button in the bottom left of the desktop and in the search dialogue type ‘regedit’

This should find the regedit.exe program and if you click it from the list, the program will open.

 

 

In the Registry Editor window that is opened, expand the folder for HKEY_CURRENT_USER to find the subfolder for Software.

 

 

 

Within the Software folder, scroll down to find the folder called ‘SolidWorks’ and expand it. This folder contains multiple folders that control different aspects of SOLIDWORKS on your machine. There are separate folders listed here for each different version of SOLIDWORKS that is installed on the machine. In the imager to the right, you may see that I have multiple versions (2012,2013, and 2014).

It is always advisable not to make permanent changes to the registry without first checking that they will not damage your system. As such, at this point you can right-click the folder that represents the version of SOLIDWORKS that you want to reset (in this case 2012), and select to Rename the folder.

 

 

 

Rename the folder to something recognisable as shown in the image to the right by adding a suffix to the name. This ensures that the folder will not move when the folders are next sorted alphabetically.

 

 

 

 

 

 

 

 

 

 

 

Now that the Registry folder for that version of SOLIDWORKS has been renamed, when the software is next started and attempts to read the registry it will be unable to locate it. This forces SOLIDWORKS to create a new registry folder with a fresh set of the default registry keys in it, essentially resetting the software options to what they were when SOLIDWORKS was first installed. When launching SOLIDWORKS for the first time after renaming this registry folder, you will be asked to agree to the end user license agreement and treated like a new user.

 

 

If you would like to check the Registry Editor again at this point, either by opening a new session (as per step 1), or by selecting View – Refresh (f5) in the menus of the Registry Editor, you will see that a new folder has been created with the same name as the original folder that you renamed.

This is an important point to make because having the new copy and the original renamed folder allows you to revert back to the previous settings should the generation of a new registry folder fail to solve any issues, or if you would like to revert back to your previous settings. The process for reverting back is very simple. Ensure SOLIDWORKS is closed, delete the ‘new’ registry folder created in the above steps, and then rename the original folder back to its original name.