How do I reference the diameter of a previously created hole?

[boylini]

Hi everyone.

I want to make a part with two intersecting holes. The first one is threaded with a 3/8 BSP thread, and the second hole is just a normal unthreaded one with the same diameter as the first.

Normally, if I was making two unthreaded holes with the same diameter I would define a parameter called 'holedia' or something and link both holes to this parameter so I can change it easily if I want; no problem.

But because this time it's a threaded hole, I can't specify the diameter. I don't know what it is because Inventor just looks up '3/8 BSP female thread diameter' in some table. So what do I reference as the diameter of the second hole?

At the moment I'm just looking up a chart of BSP threads on the internet and entering the major diameter manually, and this works although it's a bit of a hassle. But if I wanted to change the hole to 1/2 BSP; I'd have to go back on the internet and find the new diameter to use for the second hole.

There must be a way to 'parameterise' the Inventor-generated diameter of the first hole, and then reference this for the second one, isn't there?

I tried making a driven dimension linked to the first hole and referencing this in the second, but this didn't seem right and it wouldn't update itself when I changed from 3/8 to 1/2.

Please help! I think I must be missing something.

Thanks

[JDMather]

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@boylini wrote:

 .... entering the major diameter manually.

Thanks

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Major diameter?  That doesn't sound right.  Shouldn't it be the tap drill size?

I just created a threaded hole.

Started new sketch and Project Geometry the circle.
Created driven dimension and took note of the dimension name.

Created new standard hole and set size to the driven dimension.

Changed the original threaded hole and the driven dimension hole updated as expected.

[Curtis_Waguespack]

Hi boylini,

Edit: JDMather was quicker than I was, but we've described basically the same steps. As for his point about tap drill size, you'll find that listed  in the Document Settings  along with the Major diameter.

Give these steps a try, I think it will do what you're after.

Go to the Tools tab > Document Settings button > Modeling tab, and set the Tapped Hole Diameter setting to Major.

• Then create your first hole.
• Then create a sketch for your second hole, and use the Project Geometry tool to project the first hole into the sketch.
• Then place a Driven dimension on one of the projected end lines of the hole as shown.
• Then sketch your center point for the placement of the 2nd hole (I've used a construction line in the image below).

Then, in the Hole tool, simply reference the Driven dimension as shown:

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[boylini]

Hey thanks a lot for your help guys.

This is pretty much what I thought I should do, although it doesn't work for me.

I tried what you said in a new file, and I still get the same problem.

I made an M8 tapped hole in a block, then projected it in a new sketch and noted its dimension number (d9). I made a second hole with d9 as its dimension and it worked fine:

So then I went in and changed the tapped hole to M6. This hole changed size obviously but my second hole remained at the bigger size:

What have I missed??

If I edit the sketch for the second hole and examine the projected geometry, it still shows the old diameter of 6.647mm (which would be correct for an M8 hole).

However if I drag up a new driven dimension from the exact same points as the other one, this one shows up 4.917mm (which is correct for an M6 hole).

Also, I don't quite understand what changing the Tapped Hole Diameter from Minor to Tap Drill does? Does this just change how the hole is represented in Inventor?   Surely it won't affect how the second hole relates to the first?

Any thoughts?

[Curtis_Waguespack · Accepted solution]

Hi boylini,

After updating the first hole you might need to go to the Manage tab and click Rebuild All to ensure that the change has been recalculated all the way though.

Also the Document Settings option I mentioned simply changes the hole in the model to be the value you select. So if you intend for the second hole to match the major diameter of the first you'd want to change that setting as such, otherwise you'd get the minor diameter when projecting the first hole into the sketch of the second.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Curtis_Waguespack]

Hi boylini,

I just noticed that if you create a sketch on the end of the first hole and project it, and use it as a refrence in hole2, then the update is more reliable/automatic. You can then just turn off the visibility of the reference sketch.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[boylini]

Edit: Yeah you beat me to it, different ways of doing the same thing seem to produce inconsistent results.

Hi Curtis. 

Rebuild All did it! I never even knew that existed. I certainly still have lots to learn..

Interestingly I thought I had it figured out - If I selected specific points of the projected geometry then it did work without needing to be rebuilt. Very strange that this would make such a difference.

Re the tapped holes diameter, does that Document Setting apply across the entire part, or can I set it for one hole only? If so, how do you check whether a particular hole is using minor/major/tap dimensions?

Is it possible to apply this to holes I've already drawn? I have Inventor 2013.

Thanks again for your help.