Seperate complex single-body part into many bodies

[124475Tilman]

I've designed something, but unfortunately, all the parts of the design ended up in a single "body". Coming from SW and Fusion, this is a bit confusing, as this feature ("disjoint lumps") is new to me, and I'm confused as to how to separate the part into multiple solid bodies when there's no clear way to cut it using eg. the split tool. Is this possible?

Is there a single feature to do this or even a workflow? I need the parts to be in separate bodies so that I can assemble it and eventually 3d print it.

I've attached the file I'm having problems with.

[89198826955]

press the "new body" button

[124475Tilman]

Thanks for the reply however this doesn't solve the problem--It breaks the file and if I attempt to accept it regardless, it still only leaves me with two bodies instead of 14 separate bodies

[JDMather]

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@124475Tilman wrote:

 Coming from SW and Fusion, this is a bit confusing..

Is there a single feature to do this or even a workflow? 

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I didn’t look at your file, but the correct technique is to do it Exactly the same as in SolidWorks and Fusion 360.  New Body or New Component when creating.

The difference is that Inventor also permits Disjointed Lump bodies (that can be advantageous) if you don’t take explicit control.

You might be able to Edit Feature and take this control if you haven’t created dependencies that would cause to fail, or you might be able to Split what you have (same as in SolidWorks and Fusion 360). I am not at my Inventor machine to check your file at the moment, but I will check later if Edit Feature as suggested by @89198826955 or Split does not work for you.

[124475Tilman]

The issue is that, as far as I can see, a single extrusion can *only* form a *single* new body. For example, the keys are all extruded in one go despite being disconnected. In Fusion, this results in Body1, Body2, ... while Inventor only creates a single body. Even if I set the extrusion mode to "Create New Body" it still only creates a single body containing the extrusion, rather than multiple ones.

This is particularly annoying in the keyboard example I am working on, because from a time-spent and "cleanliness" perspective, it is quite cumbersome to extrude each key individually.

[89198826955]

creating an array press this button

[124475Tilman]

I've tried again, and instead of extruding multiple keys at a time, I extruded one and then patterned it as @89198826955 recommended. Unfortunately, once they are separate bodies, I can no longer reliably feature-pattern on them--when the extrusion is *subtractive*, it lets me select multiple bodies and pattern the holes, but when the extrusion feature is *additive* the gui does not let me select multiple bodies to be considered, and all the circular pattern copies end up in the original body:

I've attached my latest attempt

[89198826955]

what is your solution?

fast or good?

 Fast: Suppress array element Right mouse button, select "suppress"

[89198826955]

another solution:

designing one button with one body

designing another button with a second body

then we make an array of bodies

[124475Tilman]

Thanks for the replies, but none of these methods are really satisfactory when compared in efficiency to eg Fusion 360's method of operation. The challenge in this particular exercise is that there is collection of slight variations of a patterned element, and Inventor is apparently unable to deal with this. Specifically, most of my problems could be solved if it were possible to extrude pattern elements that automatically join bodies that they intersect, rather than either forming new bodies or staying in the original (disjoint) body.

[johnsonshiue · Accepted solution]

Hi! Indeed, Fusion considers separate solids as different bodies. In your case, you start with a sketch with disjoint profiles. Th result is a solid body with disjoint lumps. All the following features are added to the same solid bodies.

Inventor does support multi-solid body workflow and also separate disjoint lumps.

In your case, if you start all over, you will have to extrude the profile one at a time (New Solid option) to create the individual solid body.

It is indeed unintuitive to separate disjoint lumps into solid bodies. There is a workflow to help. Once you are done with disjoint lumps and you want to separate them into solid bodies, you may count how many lumps you have. Let's say it is 'n.'

1) Create a rectangular pattern of the body -> Create New Body -> set number of occurrences = n and distance to 0. You will have solid bodies overlapped one another.

2) Go to Solid Bodies folder -> right-click on each solid body -> Hide Others.

3) Delete Face -> Lump selection -> pick the unwanted lumps in the solid body. Repeat step 2 and step 3.

Many thanks!

[tomasz.sztejka]

Ehm... What are You trying to do? Should the produced keyboard really be made a separate, different keys each designed separately or an assembled set of same keys manufactured as parts? If second You should rather design each key (or two or three keys, the full and half-tone) as one multi-body part, then derive from it three parts, each made of one of the bodies, and then create the assembly made of all of them.

[124475Tilman]

This is exactly what I needed! Thanks!

Still a shame that such a un-intuitive process is required for such a (in my mind) simple operation. Clearly the software can already identify the different solids that compose the disjoint lumps (in the delete face feature) so it should be trivial to have a "Explode Solid Bodies" feature which--like the delete face feature--lets users select parts of disjoint-lump solids and separate them into new bodies (basically the reverse of the "Combine" Function).

Is there a place where I could request this feature?

[SBix26]

Inventor Ideas forum is exactly what you are looking for.  You can search there to see if such an idea already exists and lend it your support, or create a new proposal.  Either way, come back to this topic and share a link so others can add their votes.

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Sam B

Inventor Pro 2024 | Windows 10 Home 22H2

[124475Tilman]

Looks like there's nothing new under the sun. Variations on this functionality have been under suggestion for almost a decade:

https://forums.autodesk.com/t5/inventor-ideas/separate-solid-bodies/idi-p/6253275

https://forums.autodesk.com/t5/inventor-ideas/improved-multibody-tools-delete-body-fill-void-and-iso...