Hex Holes Library

[v.ibanescu]

Hi guys,

we are using a lot Hex holes to our products that have, for us, standard dimensions. Since you don't have the option in Inventor to generate directly hex holes, I want to ask you if there is a possibility to crate a library or a function that has a drop menu where I can select from a list of standard hex holes the one I need. 

For example we use a lot hex holse that have the following dimensions: 6,2 / 7,2 / 9,2 / 11,2 mm. So it will be perfect if I had a function with drop menu from wich I can select one of these values. 

Thanks a lot! 

[CCarreiras · Accepted solution]

HI!

You can do iFeatures and apply that iFeature in the parts:

Tip: you can have a parametric iFeature, so you can have only one with selectable sizes

If you will apply the feature in a sheet metal part, maybe it's better to create a punch to place it on the model based on sketched points (more accessible and faster)

[CCarreiras]

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@v.ibanescu wrote:

Hi guys,

... Since you don't have the option in Inventor to generate directly hex holes... 

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HI, when you say that, have you tried this?

[v.ibanescu]

yes :)...this was not my problem, maybe I didn't explain it correctly, I know how to draw the hex in a sketch, i just wanted an option to have the hex holes directly, without drawing them in a sketch.

[CCarreiras]

OK, good... so my approach is to use "polygon sketch + extrude" to create iFeatures, as I suggested above.

[CGBenner]

@v.ibanescu @CCarreiras 

There are several Features in the Content Center standard library under Features.

In the Part environment, you can insert these using Tools\Insert (shown below).  You select a surface and are then prompted for the parameters to define the size and depth.  I assume you could also create and publish your own to a Read\Write library... but I don't know how without a bit of research.  🙂

[JDMather]

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@v.ibanescu wrote:

For example we use a lot hex holes...

I would simply create a Punch tool for this.  Then you can place the hex holes as easily as placing cylindrical hole features.

There is one trick - you need to temporarily toggle the part to Sheet Metal (Environments>Convert to Sheet Metal) and back again after placing the hex holes.  It doesn't matter that the part isn't actually sheet metal, but you have to fool Inventor.

A Punch tool is simply a special iFeature.

[v.ibanescu]

this is actually not a bad idea, I just have to figure it out how to build my own library for our standard hex holes. Thank you! 🙂

[v.ibanescu]

so, I figure it out how to make my IFeature for the hex holes, now my next question is, how can I change the name? After I crated the IFeature, I changed the name in the iProperties to "6kant_Stahl", but when I insert the feature into my part, in the tree it apears as iFeature38, and not "6kant_Stahl", do you maybe have any tip how to change this? 

Thank you! 

[CCarreiras]

When you create the iFeature, it will create a file:      something.ide

and probably is on the default folder:

C:\Users\Public\Documents\Autodesk\Inventor 2023\Catalog (case of an iFeature)

Or

C:\Users\Public\Documents\Autodesk\Inventor 2023\Catalog\Punches\ (case of a punch)

No matter the name you gave it, when you apply the iFeature in a part, it will always be called: iFeature(number), like  an Extrusion will be called by Extrusion(number), and so on.

Well... you can Rename it after placing (not very good solution but....)

This is a good topic to ask in Inventor Ideas: iFeature name in the browser.

Another theme.... if you are using sheet metal, using punches is usually better to use than iFeatures, but if you are creating a solid part, when you turn it to a solid to sheet metal, only to apply a punch, this will add a bunch of sheet metal specific parameters to the part. when you come back to solid, you can't delete those parameters, so you have to stay with that "trash" on the part. In my case, since I use the Thickness parameter to run some iLogic rules to separate solids from Sheet metal in an assembly.... i never convert a solid to sheet metal if it is not a sheet metal part. In your case, do what it's better for you.

Tip: You can have the same feature as an iFeature and punches and apply each one when you are in a solid part, or sheet metal part. basically, a Punch is an iFeature with an extra point.