Custom Hole Sizes In SolidWorks
The SolidWorks hole wizard is a useful tool. It comes ready-to-use with a range of pre-defined hole sizes from a wide range of standards. You also have the facility to add your own custom hole sizes should the need arise. This tutorial describes the necessary steps on how to create custom hole sizes in SolidWorks when using the hole wizard.
I have created a simple cylinder part in SolidWorks. I would like to be able to run an ISO standard M4x0.5 tapped hole through the centre of the top face of this cylinder. To do this, I have opened the hole wizard and selected the bottoming tapped hole option. I have then selected the ISO hole standard and have selected bottoming tapped hole as the type (again). The next step is to select the size, I have gone through the size options but the only size which is close to M4x0.5 is M4. My thread size chart confirms that the ISO standard for M4 is in fact M4x0.7 – what now?
The answer is of course to customise your SolidWorks toolbox and create a new hole size. There are two schools of thought when doing this, some people will recommend you should copy and existing standard and make your customisations and others will tell you to just modify an existing standard. I’m of the opinion that if you’re adding a size to an existing standard (i.e. needing an ISO size that’s not already included in the ISO standard within SolidWorks) then you should just go ahead and make those modifications. If, however, you’re adding something completely new like a BSP hole size then it’s probably best to start afresh with a new standard – (I shall cover this technique at a later date).
To make modifications to your SolidWorks toolbox, you need to open the toolbox settings wizard. This is located in the SolidWorks Tools in the SolidWorks directory on your Start Menu:
Once you’ve opened the toolbox settings wizard, you will be presented with a screen like so. You need to click on option one which is for making changes to the hole wizard data:
You will then be presented with all the available hole wizard series and data. We’re interested in ISO bottoming tapped holes in this instance; so from the tree on the left hand side, expand ISO, then expand tapped holes and finally select bottoming tapped holes. This tree follows the same hierarchy as the hole wizard does in SolidWorks:
The table to the right of the window contains all of the hole sizes available to SolidWorks. To add a size, click on the + symbol at the top left corner and then fill in the required data:
Once you’ve pressed OK the new size will be appended to the bottom of the table:
At this point you’d think you’re done. But there’s actually and important step which needs to be completed first – this is where a lot of people tend to trip up. You need to click on the thread data option at the top on the left hand side of the thread size table to add the rest of the information required by SolidWorks for this new thread:
You will then be presented with another table containing more detailed data about all the available hole sizes. Similarly to adding a hole size, you need to click on the + symbol at the top left corner of the table to add new data to it. Here’s my example data for my new M4x0.5 hole size:
Hopefully you can see how this works, I have added the name of the hole size into the size column, then added the thread diameter, advance, the internal and external minor diameters and the tap drill size. This is where things begin to get a clunky in my opinion – it seems that the thread description is a duplication of Size, the same goes for fullsize. Threads per unit appears to be a duplication of Advance and Series isn’t populated in any of the default data, but the form wont validate if any of the fields are null so I just put the hole size in that field. I grabbed all the data I needed from this chart.
However, once you’ve added all the required information, you should be able to see the new record at the bottom of the thread data table:
The last step is to save all the changes you’ve made to the toolbox by pressing the save icon at the top left corner of the window:
Now, when you return to SolidWorks your new hole size should be ready and waiting for you in the hole wizard:
And finally, just to prove that it was worth all the effort. When you create a drawing of the part and dimension it, you get the full set of data needed for your manufacturer to insert the hole: