Separating Disjoint Bodies Into Parts

[Anonymous]

I'm new to Inventor and I'm having a bit of trouble doing something I figured should be pretty basic.

I have a solid that I have cut up into multiple disjoint pieces using revolve cuts with a tolerance I specified in the sketch by giving the revolve profile a thickness. So now I have a "single" solid, but it is really separated into a bunch of pieces by empty space. I just want to make all of these disjoint pieces into separate parts. I guess making them into separate solids would be the first step. I tried making a revolved surface at the center of the revolve cut but I can't use that to split the solid. It appears you can't split a solid through a disjoint space. Is there any way to do what I'm trying to do?

Thanks!

[Anonymous]

welcome to the forum,

assuming that you are using Invetnro 2010 or later, you'll want to use the New Solid button to create each solid as a seperate solid body.

here are a couple of youtube videos that show the process for working with multibody parts and making them individual parts:

http://www.youtube.com/watch?v=11dyV4InbmI

http://www.youtube.com/watch?v=iDRotf2Is2g

[JDMather]

Find the red End of Part marker in the feature browser.
Drag the red EOP to the top of the browser hiding all features.
Save the file with the EOP in a rolled up state.
In Windows Explorer right click on the filename and select Send to Compressed (zipped) Folder.
Attach the resulting *.zip file here.

[Anonymous]

That's not quite the issue. The pieces I need separate have to have a very specific bounding shape and they have to fit together. The only reasonable way I can think of doing it is making my bounding/total body, then revolve cutting my very specific grooves into the solid thereby splitting it up in separate chunks. There are two issues with using the split command: -For some reason, I can't figure out how to split on multiple surfaces into many bodies at once. Solidworks can do this so I hope Inventor can. I have 50 cuts so I don't want to have to split each one manually. -The other issue is that the splitting cut needs to have a "thickness" that it removes, thus creating a tolerance that will allow the disjoint parts to fit back together when they are physically made. Two ways I can think to do this is either to make two very close splits for each cut (making 100 cuts, see above) and delete the solid formed between them or to try to split all the parts flush THEN revolve cut a thickened copy of the split profile. I did the revolve cuts first and that makes Inventor return an error when trying to split down the empty space. The biggest issue is being able to split on all surfaces simultaneously.

[Anonymous]

without the files (as JD suggested) or at least a screen shot, I can't completely understand the issue, but typically I use the Combine command to "machine" one body from another, and then use the Thicken/Offset command to create the tolerance.

Or you might revolve the splitting surface, and then use the Thicken/Offset command to build a new solid body to the specified tolerance, and then use the Combine command to cut it away from the original solid body.

I think the part of what you're running into is a limitation of the Split command, for some reason we're not able to split a solid more than once with the same surface, not sure why. So it might take a different strategy than you've used in the past, but it can be done.

[JDMather]

Find the red End of Part marker in the feature browser.
Drag the red EOP to the top of the browser hiding all features.
Save the file with the EOP in a rolled up state.
In Windows Explorer right click on the filename and select Send to Compressed (zipped) Folder.
Attach the resulting *.zip file here.

If your file is proprietary simply make up a dummy file that exhibits ALL the behavior of your proprietary file. So easy!  So logical!  We spend all this time learning to communicate with geometry - let's communicate with geometry.

[Anonymous]

At JD. My apologies, I somehow glazed over your first post thinking it was describing how to end a part earlier in order to separate out a solid. Forgive my stupidity.

As you have predicted, it is somewhat proprietary. I don't have the time or tools to make another model right now (nor do I have the original files anyway) BUT there is a youtube tutorial for Solidworks depicting a similar idea! I planned on posting that anyway after seeing that my words weren't clear.

http://www.youtube.com/watch?v=yQNVmaXt0_E

The actual details and cuts of my project are different but this is in the same spirit. You start with a regular solid, make a cut profile, revolve that cut, then circular pattern it about the symmetries of the solid. In the end result you end up with a bunch of pieces you can touch up then send to be made that will fit back together to form the original solid and twist/slide about the cutting surfaces. It's a twisty puzzle, like a Rubik's cube.

[Anonymous]

Also, like the video, there are actually only a couple of unique pieces created and the rest are duplicates. Of course the technique for "separating" that I am looking for applies to other more general cases (i.e. where there are no duplicates) as well. In this case I would just pick out one copy of each part and save it as a separate part, then send those to have a number of copies of each made. The details of how to create an assembly file replacing each "duplicate" with just a copy of the same part file is another story entirely (and also not really necessary) so let's ignore that for the moment.

[JDMather]

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@Anonymous wrote:

... BUT there is a youtube tutorial for Solidworks depicting a similar idea!

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I am quite familiar with SWx.  Attach your ipt file here.

[Anonymous]

Like I said, I don't have an ipt to upload (I am not at my Inventor machine) but if you take a look at that video I linked to it sums up the idea.

[Anonymous]

I think this explains the issue:

You might expect the result to be six solids, but you actually end up with just 2, each with 3 "lumps". And Inventor will not allow you to split the disjointed lumps apart with the split tool.

[Anonymous]

Close..but not so much. That I'd expect since its one surface. But now say those were separate surfaces (no connecting pieces). How could you split them all without manually splitting each one? Solidworks let's you select multiple split surfaces to simultaneously split. A similar but separate problem is say that surface was actually thick and subtracted from the block. Then you'd have a bunch of disjoint blocks (with air gaps between them) that Inventor interprets as one solid. How do you make it recognize each block as a separate solid? Even if you could do a bunch of splits simultaneously, you cannot split down the middle of an air gap for some reason.

It's two related problems. In one (Issue [#1]) you start with a single solid and want to divide it into many solids using many surfaces at once (this is what the video shows).

The other (Issue [#2]) is you start with a "technically" single solid that is really a bunch of disjoint chunks with air gaps between them and you want Inventor to recongize each chunk as a separate solid.

If the [#1] was easy to do, you could do it then manually thicken the cutting surfaces then extrude and end up with the result of [#2]. I am sorry that this is so hard to encode in language...or even video it appears...I guess I just think its simple because I already know what I mean. I will upload example ipt files as soon as I can, but that might be awhile if anyone thinks they understand please do provide input. Thank you for the attempts thus far.

[Anonymous]

BMiller63 is very very close to the problem though and

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@Anonymous wrote:

And Inventor will not allow you to split the disjointed lumps apart with the split tool.

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wraps up one of my issues. The other is that you can't easily make a whole bunch of splits at the same time. If you could make a whole bunch of splits at the same time, the first issue wouldn't really be a problem since in BMiller63's example you could just make one surface, linear repeat it, then do all the splits at the same time. If you then wanted to add air gaps between the solids (for physical tolerances) you could thicken the cutting surface, linear repeat, then extrude cut.

Basically you have this (A): http://www.cs.ru.nl/~ths/rt2/col/h2/colorcube.jpg

and want this (B): http://members.peak.org/~jeremy/bigfun/netscape_216.gif

where each little cube is a SEPARATE solid. I can make (B) from (A) by extruding and linear/circular repeating, but the result will be called a "single" solid by Inventor. So issue [#2] from my last post is that I already have (B) and want Inventor to recognize the parts separately. Issue [#1] from my last post is the case where I have (A) and have patterned a bunch of surfaces which I want to use to split (A) into something like http://www.frank-tclark.com/Professional/Papers/ColorHCW/RGB-Cube.PNG with each cube a separate solid. I would then pattern an extrude cut (thickened copies of the cutting surfaces) and cut on all the new solids to reach (B).

Of course my case is more complicated than a big cube separated into little cubes but it wraps up the idea. My project is making a puzzle similar to http://www.youtube.com/watch?v=yQNVmaXt0_E and having air gaps (tolerance) so that it turns easily without locking up. The key of course is that each chunk must be manufactured as a separate part, and you can't just give the manufacturer a single assembled puzzle to make or print all at once assembled.

[Anonymous]

to be clear, there are methods to get the end results you're after, but not using the method you are attempting.

for the record I think it should work as you expected it to.

you might go here and request it:

http://usa.autodesk.com/adsk/servlet/index?siteID=123112&id=1109794

[JDMather]

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@Anonymous wrote:

to be clear, there are methods to get the end results you're after, but not using the method you are attempting.

for the record I think it should work as you expected it to.

you might go here and request it:

http://usa.autodesk.com/adsk/servlet/index?siteID=123112&id=1109794

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Yes - I agree.  It would be nice to be able to use the SWx method in Inventor.
The Inventor solution will likely involve Derived Components and Sculpt technique.

[johnsonshiue]

Hi! I am assuming that there are multiple disjoint lumps in one single body in the file (Solid Bodies folder = 1). Split command requires the split tool intersecting the lumps. In your case, it will be difficult to find a split tool (surface or sketch) helping separate the lumps.

There is a less well-known workflow you can try. It should work for you.

Let's say you have 4 disjoint lumps.

1) Launch Rectangular Pattern command -> pick the 4-lump body -> enable Pattern a solid option -> enable Create new bodies option -> pick X axis as direction -> set distance to 0 and set number of occurrences to 4 -> OK.

You will get 4 bodies and each with 4 lumps.

2) Go to Solid Bodies folder in the browser -> expand -> right-click on Solid1 -> Hide Others.

3) Launch Delete Face command -> enable Select lump or void mode -> pick the unwanted lumps in Solid1 -> OK.

4) Repeat step 2 and 3 for other bodies.

Let me know if you have any question.

Thanks!

[Paul.Normand]

There are two videos posted on the Wiki that deal with multi-body solids.

The first one posted here provides an overview.

http://wikihelp.autodesk.com/Inventor/enu/community/Videos/Show_Me_MultiBody_Parts

The second one posted here shows the workflow to create multiple (disjoint) bodies on forward creation or after creation using Edit Feature.

http://wikihelp.autodesk.com/Inventor/enu/community/Videos/Create_multiple_disjoint_solid_bodies

Hope that helps.

Best Regards,

Paul Normand

[Anonymous]

paul, can you comment on the process of using the Split command to generate multiple disjointed bodies?

the links you provide don't address that.

[Paul.Normand]

If the bodies don't touch, then the split command fails to create new bodies. If you can't use Edit Feature and select New Solid (on the base feature for a required body), then the method that Johnson suggested is the only way I know that would work.

I can create a video of the steps he suggested and post if needed.

Regards,

Paul

[Anonymous]

Thanks Paul,

Somehow I missed Johnson's post last time, but his method is the same as is shown in the youtube video I posted at the beginning of this thread, only that video uses the circular pattern, and he adds the delete face trick.

It's the ability to chop up and seperate solids that Inventor lacks (and apparently Solidworks has). I can think of a number of workflows where this would helpful. It really should be considered for the future.