Cut & Paste Solids to Create Multi-Body Part

[Anonymous]

After migrating my project from MDT2009 to Inventor 2010, every solid body in MDT became a part file in INV.  If I were modeling from scratch, some of the .IPTs should be multibody parts.  Is there any way to cut & paste a solid from one part to another to create a multibody part?  I’m not talking about deriving a new part from the source parts.  The end result should be a multibody part with all sketches intact and all solids fully editable, as if I had modeled them as a multibody part right from the beginning.

I’ve attached a simple example of two separate parts that should be combined into one multibody part, as shown in the .JPG file.  Can it be done without deriving the parts?

Thanks - Mike

[JDMather]

What about Copy and Paste?

[Anonymous]

I've tried copy and paste, but Inventor 2010 does not seem to support copying a solid from one part into another part to create a multi-body part.  I wish it were that easy!  That's why I'm asking if there are other methods I am not aware of (besides deriving yet another part file).

Yes, the multibody functionality would be greatly improved if I could "copy and paste" a solid from one part into another part, and then delete the exteraneous part.  Are you saying that you can do this (with all sketches intact)?

- Mike    

[JDMather]

When you create a multibody part, say with an Extrusion feature, you must click the box for new solid.
If you then additional features you must tell Inventor which of the two solid bodies to apply the feature to.

Copy and paste (the hardest step is figuring out how to place the Paste so that it does not need to be moved).

Now the features and sketches from the second part are in the first part, but Inventor has not yet been told to create New Solid.

Edit the logical base feature of the new solid and check the New Solid box.
Edit child features and Ctrl unselect the first solid body and select the second solid body.

Save the multi-body file.

Delete the file from which the geometry was copied.

The question has to be asked. "Why are you doing this?" (especially since you cannot (will not?) use Derived Component)

A lot of MDT and AutoCAD users are inexperienced with a part is a file concept.
If you are simply trying to mimic AutoCAD file structure  - this is not a valid reason.

If multi-body would aid in editing - this is (might be?) a valid reason.

[Anonymous]

I appreciate the comments, but I'm not a 3D newby trying to recreate the MDT part heirarchy.  I've been using the "part is a file" concept with Catia 5 for 7 years at my job.  Inventor is my personal CAD software and I've made extensive use of derived components with Inventor.  But there are certain times when a multibody part is the preferred method.  Multibody parts were a great advancement in Inventor's functionality!  But the migration from MDT has resulted in every solid being a part.  There are several parts that would have been multi-body parts had I modeled them in Inventor instead of MDT.

Here's what I found after experimenting with part files:

1)  You can COPY the .ipt from the model tree but will be unable to PASTE it into another part

2)  You can't COPY a solid no matter how hard you try

3)  You can COPY multiple features from a solid in one part and PASTE them into another part, but they will become features on the existing solid (in the second part) rather than a separate solid.

It sounds like you are suggesting that I create a second "placeholder" solid in the original part.  Then I can copy features from the other part into the first part and tell Inventor to add them to the second solid body.  I will try that approach and the 2nd method that you suggested.  These work arounds are more involved than I would like, especially since Inventor prompts you for new sketch planes when pasting features (and if you pick the wrong one, the feature moves).

I also plan to try the following:  Combine the solid bodies in MDT before migrating to Inventor; then the combined solids should be in one part file at least.  Copying solids is so easy in Catia 5.  I've noticed that Autodesk tends to add Inventor features that mimick Catia 5's functionality, so maybe someday...

Thanks

[JDMather · Accepted solution]

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@Anonymous wrote:

It sounds like you are suggesting that I create a second "placeholder" solid in the original part.  Then I can copy features from the other part into the first part and tell Inventor to add them to the second solid body. .... I've noticed that Autodesk tends to add Inventor features that mimick Catia 5's functionality, so maybe someday...

Thanks

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No. 

 I'm suggesting using the same logic Inventor uses in creating multi-body solids.

Copy the features from one part into another.
As you have found Inventor adds these features to the second solid body because there is no option in Copy/Paste to tell it to create a New Solid.
Simple edit the features once copied and click the New Solid box.
Edit child features as needed.

How long into the future we will have to wait to see this Copy/Paste gain the New Solid functionality is anyone's guess.  It might not be so much a case of copying someone else's functionality as it is simply a case of adding obvious functionality as the product/feature set matures.  In the end geometry is geometry - only the interface used to obtain the geometry is different.

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

I recommend you provide link back to this discussion - they like concrete examples.

[Anonymous]

Yes, I will try that method.  The example I have in mind is an engine crankcase.  Due to the complexity of this shape, I modeled it as two separate solids in MDT to make it easier to edit.  But the real crankcase is still one part and it's odd to see them separated as two parts in Inventor.  Hence the desire for a multibody part in this case.

I've marked this "accept as solution".  Thanks. 

[rdyson]

Why not boolean union them in MDT???

[Anonymous]

Try this:

place both parts in an assembly file, constrain them into proper place,

then edit one of the parts,

then use the Copy Object command, to copy one of the parts into the other.

it'll come in as a seperate solid body.

[Anonymous]

Too busy today, but can't wait to try that tomorrow.  That idea sounds like a winner if there are no hidden drawbacks. I will report back on these new methods after I try them out.  Thanks.

[JDMather]

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@Anonymous wrote:

  That idea sounds like a winner if there are no hidden drawbacks. 

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I thought your whole problem description was how to preserve multi-body solids?

The end result should be a multibody part with all sketches intact and all solids fully editable, as if I had modeled them as a multibody part right from the beginning.

[Anonymous]

You are correct - to create and preserve a multibody part.  Is that not what the author described when he suggested editing the first part in an assembly, then pasting in a part object as a second solid to create a multibody part?  Will I be able to delete the second part file afterwards, or are we back to deriving parts?  That was my concern - that pasting in the object would function as a derived solid without sketches.  I haven't tried it yet, so I don't know the answer. 

The boolean approach in MDT also sounds promising.  Your suggestion is also good but may be more difficult for the crankcase example where there are a lot of sketches.

Thanks all,

- Mike   

[Anonymous]

oh, sorry.

My solution will not bring across sketches, therefore is no solution if that's what you need.

[JDMather]

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@Anonymous wrote:

....Is that not what the author described when he suggested editing the first part in an assembly, then pasting in a part object as a second solid to create a multibody part?  Will I be able to delete the second part file afterwards, or are we back to deriving parts?  That was my concern - that pasting in the object would function as a derived solid without sketches.  I haven't tried it yet, so I don't know the answer. 

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Huh? I'm the author of those steps and I tested them before posting the steps.

[Anonymous]

I was referring to BMilller63's post #9, which is somewhat different than your process.  BMiller63 later realized that his approach does not include the sketches, so it's no good for me.

I tried copying features from a solid and pasting them into another part, then editing the feature to "make new solid".  That aproach works, but INV prompts you to select a sketch plane for each of the new features.  Unless you've already set up duplicate sketch planes to match the original solid, the features start to move around.  I was able to do it for the simple example in my original post, but it was almost the same amount of work as creating the second solid from scratch.

My crankcase example has dozens of sketches and some of the sketch planes are based on faces at compound angles.  Copying features isn't going to work on that one.  I did submit an enhancement request to add a buttton for "create new solid" when copying features, or just let us copy and paste a new solid.  I hope to see that feature someday.

For my crankcase example, I will boolean the two solids together before migrating from MDT.  I assume the .ipt version will have two solids that are also booleaned.  That will work fine for me.

Thanks everyone for your suggestions.          

[rdyson]

Without seeing your files it's impossible to say for sure, but probably the MDT part will import as a single body.

Which raises the question, if you need two parts, why not have two parts?

If you want one part, why multiple bodies?

[Anonymous]

As stated in post #7:

"The example I have in mind is an engine crankcase.  Due to the complexity of this shape, I modeled it as two separate solids in MDT to make it easier to edit.  But the real crankcase is still one part and it's odd to see them separated as two parts in Inventor.  Hence the desire for a multibody part in this case."

The crankcase is one part, but is very complex.  There was an obvious division in the grouping of features on the crankcase, so it made sense to model it as two solids.  This makes the part much easier to edit and is no problem at all in MDT.  Migrating the part to INV split the single part into two separate parts.

[Anonymous]

I know this is an old post but I didn't want to create a new one with the same problem.

Originally we received two parts from a supplier: a bent sheetmetal door frame and the bent door that fits within the frame.  The geometry allowed for the door and frame to be cut as one piece for us, bend it as one piece, install the hinges and hardware on it and then simply cut the tabs to separate the door from the frame.  It complicated matters when we had to put it in our MRP system because we ordered one laser cut piece to create two parts but we found a messy solution.

The customer has now revised the entire assembly, and these two parts are now one.  We have not, however, been supplied any new geometry for the move to one part.  Previously I had derived the assembly into a part to get the single part to order.  Now I need to combine the two parts into a single part so that the right number comes up in the BOM.  The other added complication is that we were supplied a bent file and a flat pattern file for each part because Inventor would not translate the part files in such a way that we could bend them, so we had a flat part derived from the flat assembly and a bent part derived from the bent assembly.

Is it possible to combine the two (bent or flat) solids in one part file and name it the new single part number?

[JDMather]

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@Anonymous wrote:

Is it possible to combine the two (bent or flat) solids in one part file and name it the new single part number?

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Sounds like a different problem - probably should have started a new thread.

Open one of the parts.

Derive Component the second part into the first part (as solid body).

Use Move Bodies to move second part to correct position of first part (if needed).

Combine.

[Anonymous]

I tried the Derive and it doesn't allow for it to come in as a solid- only as a Work Surface.