SOLIDWORKS Hole Callouts provide a quick way of conveying information in drawings. SOLIDWORKS provides a large library of standards for users to work from, but there may be a situation where the client has their own set of standards. In this article, we will go over the process of creating a custom hole callout standard in SOLIDWORKS to fit your needs.
We will need to modify the file called calloutformat.txt to add our own set of standards. This file is typically located in the folder file path C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\lang\english. If you are not sure where it is, go to Tools > Options > System Options TAB > File Locations and look for Hole Callout Format File in the folder dropdown menu. From there you will see the file path listed below the dropdown menu.
Before editing the file, please copy the file to a different location and begin editing there. Making any changes when working on the file in the current location will not allow you to save any changes
To create a new standard, open the calloutformat.txt file using Notepad. It is recommended that you copy an existing standard that is similar to yours. In the image below, we will be creating a new standard based on ISO. All text below [ISO] and above the next standard, [JIS] will be copied then pasted at the bottom of the file.
From here, the text between the square brackets can be used to change the name of the standard. In the example below, the new standard has been renamed to My Standard. This will be the name that appears in the Standard dropdown menu in the Hole Wizard.
When editing the values that will appear in the drawing you can input your custom values after the equal sign of the equation as indicated in the example below.
* Blind Hole COUNTERBORE-BLIND= place your values here <MOD-DIAM> <hw-diam> <HOLE-DEPTH> <hw-depth>;\ <HOLE-SPOT><MOD-DIAM> <hw-cbdia> <HOLE-DEPTH> <hw-cbdepth>
You will also notice that some of the values for callouts are encapsulated in angle brackets (<>). These values can represent symbols or values pulled from the properties of the file. A guide for the syntax can be found in a file called gtol97.sym and at the end of the calloutformat file which can usually be found in the folder C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\lang\english. If it is not found there, use the same method stated above to find where the Symbol Library File location. You can open this file using Notepad.
When you have completed editing, save the file. In the original location, rename the original calloutformat.txt file, this way, you can go back to it if needed. From there, paste the modified version into the folder. You should see the new standard pop up when using the hole Wizard.r
Creating a custom hole callout standard in SOLIDWORKS can be a bit tricky when first starting off, but once your get the hang of it, it can be a powerful tool that can streamline your company’s workflow.