Cutting a hole from another part

[c.baynham]

I wonder: is it possible to define a part such that, when included in an assembly, it cuts features from the parts already in that assembly?

To avoid an XY problem, I'll explain what I'm trying to achieve. I'd like to define a part that mounts to another one, e.g. a solid base. My part has mounting holes, and I'd like to define tapped holes in the base which match the clearance holes in the part. I know that I could simply place the part on the base then define tapped holes which mate to the part's clearance holes. However, I'll need to place this part many times and that's an error-prone step. Can I define the holes in the part somehow such that placing it into the assembly causes the correct holes to be drilled into the base?

Thanks a lot!

[mcgyvr]

Have you tried the "Bolted Connection" functionality in Inventor?

https://www.youtube.com/watch?v=7KjkCIIJmvA

Or editing the parts in the context of the assembly and projecting the existing holes to create new ones.

No "magic/easy" hole creator function based just on placing parts into an assembly though.

[SharkDesign]

The usual way to do this is to project the geometry, although that creates associative parts/sketches and they usually lead to bad news. Here's what I do to turn them into normal sketches:

https://www.youtube.com/watch?v=4NEFnn1_HBw

One thing you could try, is to create an 'ifeature' for your part if you are placing it a lot of them and then all the holes will match without you having to define the dimensions.

If it's just in this part, you can name the parameters, i.e. xHole=100 yHole=75 and then you just use these names on every sketch you do, updating the parameter updates them all.

There is no magic hole driller like you are asking though.

[cadman777]

Assembly inter-part connections is a big issue w/Inventor, and always has been. It's due to how the software works. It's not like structural steel software that makes all kinds of nice neat connections between parts with bolts, holes, welds and all.

Maybe if you go into the Inventor Customization forum, someone in there may have a solution for you using VBA or iLogic? The rule would have to locate the hole center and then transfer it into the mating part and add a hole/tap/whatever. You can do all that with a DialogBox interface and drop-down selection boxes using VBA/iLogic. I can't do the coding b/c I'm not good enough yet, but others in the Customization forum may be able to help.

This is an Inventor feature I've needed for over a decade! I'm sure I'm not the only one.

[johnsonshiue]

Hi! On top of what experts already mentioned, there is a workflow you may want to take a look. It is called Copy Object. Edit the to-be-cut part in place -> go to Modify -> expand the panel -> Copy Object -> pick the faces or entire body from the tool part. Then you will get the geometry from the other part. Use Sculpt or Split to cut.

Many thanks!

[CGBenner]

@c.baynham  Did the information provided answer your question? If so, please use Accept Solution so that others may find this in the future. Thank you very much!

[cadman777]

Never even thought of doing it that way!

Gonna have to try it next time to see how it works.

If it works, then maybe I can use it with libraries for making structural connections?

[c.baynham]

Thank you all for all these suggestions! I'll give them a try when I can and write back with what I end up doing.

[cadman777]

Hey Johnson,

I just tried this on an large assembly (platform with bolt-on railings from a past job). It works marvelously! haven't tested it thoroughly, but will try it next time I have to do this kind of thing. After all, maybe there's some hope for Inventor 'Adaptivity' in Assemblies?!

[johnsonshiue]

Hi Chris,

I am glad to hear that it works for you. Associative Copy Object is like adaptive body (as opposed to adaptive sketch or feature). Essentially, when the source body (solid or surface) changes, the adaptive body will change accordingly.

But, this is not flexible part yet. All limitation pertained to Inventor adaptive remains true to this workflow.

Many thanks!

[cadman777]

Hey Johnson,

I did a little more testing with this on a railing/platform assembly.

By accident I selected the wrong hole surfaces, but could not find any way to 'Remove' them from the 'composite' selection set. There were 15 holes selected and I needed to remove only 2 of them. Is there a way to do that in the newer versions of the software?

[johnsonshiue]

Hi Chris,

No, unfortunately there isn't much change in terms of this workflow on newer releases. Another approach you may consider is to select the entire body instead of individual faces.

Many thanks!

[cadman777]

Thanx for the confirmation.

Can't do the whole body b/c all I need are the holes.

Basically, I Copy them, then Elongate them and use Sculpt to cut the holes in the part.

Works a charm!