Have you ever wanted to add a hole type to the hole wizard in SolidWorks. In a manufacturing environment you have common holes that you use such as reams or dowels. Now you could just use the standard drill holes that are in the hole wizard BUT when you use the hole callout function in your drawings it will call them out as a drill and not a ream or a dowel. This could pose huge problems for when you go to assemble your tool. Here is a quick little way around that situation.
1.) Go to Tools > Options > System Options > Hole Wizard / Toolbox and select Configure OR go to Start > All Programs > SolidWorks XXXX > SolidWorks Tools > Toolbox Settings.
2.) Select and click on the standard that you would like to copy for your new standard. It will more than likely be either ANSI Inch or ANSI Metric.
3.) On the top of the screen you will notice an icon that will allow you to copy the standard. Once you click on that button it will prompt you to name your new standard. Name your new standard and select the green check mark.
4.) If you have successfully completed this you will notice that SolidWorks is now creating a new standard. In my case, I named my new standard “PRESS FIT DOWELS”.
5.) Once it has been created, you will now notice it on your main screen with the rest of your standards.
6.) Select your new standard and turn off everything that you do not want to keep. In my case I am turning off everything but fractional drill holes. You can see this in the next 3 images.
7.) Once you have completed this, select option 2 on the top toolbar of your screen (next to the Save button). Once you have moved to “2 – Customize Hardware” select your newly created standard.
8.) Click through the necessary screens until you arrive at a screen that looks like below. Now turn off all of the holes that you do not want to appear. In my case I only want to be able to use a 1/4”, 5/16”, 3/8”, 7/16”, and a 1/2” press fit dowel. Once you have turned off all of the ones you do not want to use, click Save and close the program.
9.) Now you will want to find the calloutformat.txt file. This is by default located at C:\Program Files\SolidWorks Corp\SolidWorks\lang\english. Open the txt file and add a standard at the bottom. To find out how to do this click here. Save your calloutformat.txt file and close it.
10.) Now open SolidWorks and start the hole wizard tool. Click on the corresponding Hole Type icon which in my case is a drill hole and in the Standard dropdown, select your new standard. You will notice that the sizes dropdown only include the hole sizes that you left checked. Note: Your new standard will only appear in the Standards dropdown on hole types that it has.
11.) Now create a drawing of your part and using the Hole Callout function (located on the Annotation toolbar) dimension your holes. You will see that the callout looks exactly like you called for in the calloutformat.txt file.
I hope this little trick will make your life easier and eliminate possible problems that you have currently come across.