Clearance and Tapped Hole in one feature

[akAMYTB]

Hi

This is a suggestion to extend the hole feature to optionally do both a Clearance Hole in one range of selected solids and a Tapped Hole in another range of selected solids, both respecting a common set of parameters. All in the same instance of the feature.

In the current version of the hole feature it is necessary to repeat the hole feature, and match their parameters manually. In turn the two features would have to be updated individually, eg. in case the size of the intended screw or bolt changes. 

Cheers - Anders

[Anonymous]

I like it, can you put it in the idea station so we can gather support? Feel free to link to it here after it is up.

https://forums.autodesk.com/t5/inventor-ideas/idb-p/v1232

[akAMYTB]

Whoops... my mistake.. here's the link 🙂

https://forums.autodesk.com/t5/inventor-ideas/clearance-and-tapped-hole-in-one-feature/idi-p/9981839

[SBix26]

I tried to vote for your idea, but the forum will not accept my vote.

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Sam B
Inventor Pro 2021.2 | Windows 10 Home 2004
LinkedIn

[LFMarshall]

likewise

[johnsonshiue]

Hi! Though it is not 100% the same, in the meantime, you could try extracting clearance hole and tapped hole to an iFeature.

Many thanks!

[akAMYTB]

I got that note from a colleague too. However, the Idea recieved one vote now from another user, so maybe voting is up again 🙂 Thanks for the support...

[SBix26]

I found a topic about the "Vote" problem in another forum, and one workaround is to right click on the Vote button and select Open link in new tab.  I just voted successfully using that procedure.

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Sam B
Inventor Pro 2021.2 | Windows 10 Home 2004
LinkedIn

[abhay.gilka]

Hi @johnsonshiue , Can you share some example of how to do tapped hole, clearance hole and counterbore in ifeature (attached file)? Thanks and much appreciate your help.

Currently we are doing this in 3 steps of hole operations and having hard time dimensioning it.

This hole feature is on cylindrical shell split into two, threaded portion on one half, clearance and c'bore on the other half.

Hope to hear a better solution. Thanks!

[James_Willo]

You are asking for a specific feature, but in the mean time I have done this many times in the past. 

Create a normal thread through both bodies

Turn on the counterbore option to add the clearance hole. 

You can probably control depth of each using parameters from other features. 

[abhay.gilka]

Hi @James_Willo ,

Attached is my file, kindly guide how these 3 hole features can be combined into one?

Thanks!

[James_Willo]

Sorry, I was replying to the OP, didn't realise it was a year old. 

Please find attached, I've done it in 2 operations instead of 3. 

[abhay.gilka]

Good attempt.. but my intent is to adjust the clearance and counterbore automatically based on the screw size

[johnsonshiue]

Hi! Extracting the features as an iFeature isn't an issue. The problem is that the hole spec is literally captured as individual parameters, not as a particular spec from the Thread table. As a result, there isn't a way to specify the spec on placing the iFeature. Also the parameters from different holes don't carry any relationship.

The only feasible workflow that I can think of is to create a part and create the drill (to drill the holes) accordingly. Then derive the drill part as a new body wherever you want to drill the combo hole. Use Move Bodies or Direct Edit to relocate the drill. Lastly use Combine -> Cut to create the hole. In this way, you can change the hole spec in the drill part easily.

Many thanks!

[abhay.gilka]

Thanks Johnson,

Quite an interesting workflow..Can you please guide me with an example using the attached ipt?Thanks!

[johnsonshiue]

Hi! I no longer have access to 2019 so I cannot share a 2019 file with you. Here is what I would do. This is a simple proof of concept you will know what I mean quickly.

1) Use Delete Face command select all the faces except the hole faces.

2) Create a Boundary Patch surface to fill the top of the hole.

3) Stitch them back to a solid.

Now you have the tool. You can derive it to wherever you need it. Then use Combine -> Cut to drill the hole.

Many thanks!

[abhay.gilka]

Thanks Johnson! I have followed your steps and  did boundary patch and stitch but couldnt convert it to a solid (please refer attached)..Kindly assist and send me file in Inventor 2022 for reference. I have latest inventor installed as well.Thanks!

[johnsonshiue]

Hi! For your case, the Split isn't needed. Please suppress it. Then delete the faces accordingly. You will only need one boundary patch at the top to turn it back to a solid body. If I were you, I would create this tool in a box instead of a cylinder to avoid the cylindrical face at the top.

Many thanks!

[sbalasubramanianJJDFU]

Hi @johnsonshiue , Can you please explain the steps after deriving the part to combine cut? Little confused on how can I correctly place the derived drill bit on sketch points? Kindly advise.Thanks!

[johnsonshiue]

Hi! Once the tool part is created, simply derive it as a body to the target part. Use Direct Edit -> Body -> Move (or Move Bodies) command to relocate the tool. Lastly use Combine Cut to create the feature. To certain degree, this process mimics what should have happened in real world.

Many thanks!