Single Inspection Dimension for Holes
I was having a hard time figuring out a good way to dimension a hole with both the diameter and depth of a hole with GD&T in a singe dimension. This dimension also required inspection so I wanted the inspection circle around the dimension and have the properties linked to the model. I did a lot of searching on the internet and did not find a good solution.
Here is my solution. please leave your comments if you have a better way to do this.
My model had a hole I needed to dimension the diameter and depth in a single inspection dimension. The hole passed through a slot and was not created with the hole wizard so when using the "hole dimension" it creates two separate dimensions.
Not what wanted.
This shows the result I am looking for. The problem with this method is that the depth of .28" is not linked to the model. if I change the feature the drawing will not update.
Create a note with a leader and attach it where needed.
***note: this leader does not act the same way as a radius or diameter leader where it points to the center of the circle. I will show you how I adjust this later but it is still a manual operation. I would love a better solution to this if you know of one.
Now if you click on a dimension it adds a link to the note that will update as the linked dimension updates.
I am about to click on the .08
You can see the link added in the note and now I am going to click on the depth dimension.
A carriage return and now I click on the GD&T box.
Here is what my note looks like with all the links.
Now I can go back to my diameter dimension to make changes. just click on the referenced dimension.
As I add the diameter symbol (or any other modifications) in the "Dimension Text" the linked information in the note is updated.
I will do the same for my depth dimension.
And add the Depth symbol.
If I click on the inspection box in the dimension only the linked dimension in the note is circled.
I want both the diameter and the depth to be in a single dimension.
If I click on the Note there is an option for Borders near the bottom of the feature ribbon.
And an Inspection Border!!!
However this will circle the entire note. :(
So put this back to 'None' when the note is selected as shown.
Instead, double click on the note so it opens up and just select the links you want circled and not the GD&T box.
With this information selected change the border to Inspection. This will only apply the boarder to the selected are of the note.
The red arrow is showing the border over the links.
And now our note looks the way we want!
I now adjust the leader of the note to align with the leader of the dimension. I have not found a way to snap or lock the leaders together or get the leader of the note to operate the way I want so please let me know if you have a better way to do this.
Now you can right click on the referenced dimensions and Hide them.
Right click and Hide.
Now that these dimension are hidden, how do I make changes in the future?
I have this command in my Drawings Flyout Toolbar
But you can also find it in the search bar at the upper right corner of your window.
With this command you can toggle notes and dimension from hidden to shown just by clicking. All hidden notes are grey with shown notes as black.
Let me know if this helped you!