Creating hole in assembly

[Anonymous]

Hi everybody,

I have created hole in the assembly from part A to part B. but when I open either part A or part B, there is not any hole on these parts!!! (see photo)

It seems the hole is just in the assembly.

Is there any way to have the hole on parts too or not?

thanks

[Sergio.D.Suárez]

Hi, When you create holes from assembly these will be created as assembly operations, that is to say as operations of machining the finished assembly for example. If you would like to have holes in the parts you must create them in the parts. Below I show you a video that you post in the forum in the thread of another partner.

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Hello, welcome to the forum. Here I show you a video with two examples. The first the easiest, you must have the boxes checked within assembly options as shown in the video to allow the associativity between the parties.
The second method is through a derived piece. A base part is derived inside the other, it is relocated and the hole is projected on the new part, finally it is extruded. When the assembly is created, note that the two parts are placed in assembly as "place gorunded at origin" (right click on the graphic window to select it)

I hope the video will be useful. Regards!

[anoor]

You've created a hole within the assembly and not the parts so it won't show up on the individual parts on a drawing. You have to create the hole within each of the parts in order for them to show correctly on the drawing.

[Mark.Lancaster]

@Anonymous 

It is possible by using this CoolOrange add-on that's free  that will take assembly features to part level

https://apps.autodesk.com/INVNTOR/en/Detail/Index?id=4113747616755499758&appLang=en&os=Win64

Currently only supports Inventor 2018 to 2020.   Not sure what version you're using.

However as others pointed out..   Out of the box it is not possible.

[johnsonshiue]

Hi! On top of what experts already mentioned, you can also use Bolted Conn to create the hole from assembly, propagating to individual parts.

Regardless, you need to think about when the holes will be drilled. Should they be drilled in the parts individually before you assemble the parts? Or, they are drilled when the parts are assembled?

Many thanks!

[Anonymous]

Hi Sergio,

When I project a line in an assembly, sometimes the color of the projected line in yellow with a specific sign and sometimes it is in blue with fix constraint (see photos I have attached). I do not know why? Is there anybody who knows the reason and the differences between these two types of projected line?

thanks

[Sergio.D.Suárez]

The difference I showed you in the video above. The yellow line is associated projected geometry, that is, if you modify the component from which you projected the line, your line will be modified and updated, since it has an associative link with the original entity.
The dark blue line is fixed geometry, if you modify the component from which you projected the line (move it to another position for example), the line will not be updated because there is no associative link with the original entity.
I hope I have been clear so you can understand the differences. regards

[Anonymous]

Dear Sergio,

I got your meaning. But the thing is not clear for me is:

when gets the projected line yellow and when is it blue?

It seems it is out of my hands when I project lines or part edges. Sometimes the line gets dark blue, sometimes it gets yellow, and I have no control on it!!!

I mean when I project a specific line, I want the line to be associated projected geometry, but strangely the line gets dark blue and it seems it is not associated geometry.

Should I follow a special way to project a geometry to be associated with the component?

Thanks

[JDMather]

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@Anonymous wrote:

It seems it is out of my hands when I project lines or part edges. Sometimes the line gets dark blue, sometimes it gets yellow, and I have no control on it!!!

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Post example files. (2 or 3 part files and one assembly file please)