SOLIDWORKS: Cosmetic Threads

Cosmetic Threads


Cosmetic threads can be a useful annotation to help manufacture parts. As a best practice, I always recommend using the Hole Wizard to create cosmetic threads it creates the correct hole size and adds the thread size automatically. All the geometric data that is required to create the desired hole is in a database that the Hole Wizard references. To access this data the only thing that is necessary is to select the standard (ISO, ANSI, etc) and the bolt or screw size. Depending on the hole type (counterbore, counter sink, clearance hole, tapped hole, etc) the correct values are referenced and used to create the hole feature.


Some customers prefer to cut a circular hole and then add the Cosmetic Thread. Also, there are a few applications where this is necessary, think about an imported body with holes that need thread callouts as an example. I have encountered some complications and confusion whilst working technical support that I will endeavor to clear up in this blog article.


The first thing that one will discover when using the Cosmetic Thread feature (found on the Insert menu -> annotations flyout) is that not all thread sizes are available when selecting any standard other than “none”. I have tested this for the ISO standard and have discovered a pattern that will demystify this behavior. I created a simple block then made several holes with increasing diameter dimensions (tangent: this can be easily accomplished by creating a single circular cut and then linear pattern with the vary pattern option) and then checked to see which thread sizes were available with the Cosmetic Thread. I then compared the findings with the Hole Wizard database, see the screenshot below, and made an interesting and rather dull discovery. The Cosmetic Thread feature uses a simple mathematical expression to determine which thread sizes can be assigned to certain hole sizes. On the left, below, you will see a table with 2 columns, first column is the hole size and second column is 1.5* hole size. This is a range that SOLIDWORKS creates and then compares to the Hole Wizard database on the right, below. All standard sizes within the range become the available thread sizes. For example, the 5 mm hole has a range between 5 and 7.5 mm if you compare this range to the last column on the right-hand side table you will see the corresponding standard threads are M6, M8, M8 x1.




What an arbitrary criteria for generating the thread size for a given hole! Feel free to check this out on your own, try the 6, 8, and 11 mm hole sizes and see what threads that the Cosmetic Thread feature makes available. You will see that this range described described above holds true. Now what if you create your Cosmetic Thread feature and it is not visible? There is a simple solution but not entirely intuitive.


For SOLIDWORKS 2016 and newer, select the eyeball icon on the Heads Up menu (shown below). For previous versions of SOLIDWORKS the eyeball icon is replaced with eyeglasses.




A list will drop down and the icon with the letters “ABC” in the left-hand column must be selected (you will know when it is selected when it has a square, grey background).


Finally, what if you would like to configure the part and need to configure the Cosmetic Thread feature? You may create a new configuration and change the Cosmetic Thread callout or configure it and that seems to work fine as long as you are changing it to an acceptable value, discussed above. Or you can create an excel based design table. All of these options work, but in some cases the design table failed to create new configurations when the user added a new configuration row if there is a Cosmetic Thread callout linked to the design table. A work around for this is to create a blank column that separates the Cosmetic Thread callout column from the table, then create your new configuration row and accept the table. Go back and edit the table to delete the blank column. See screenshot below.




This does not affect every user and I hope to see it resolved soon, but for now, this is the most efficient work around that I have discovered.



Matthew Fetke, CSWE
Application Engineer
Computer Aided Technology


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