How to unlink iParts with editing capabilities?

[Anonymous]

Is it possible to take an iPart and derive it to be its own part with all of the sketches and features retained? By that I mean fully extracting it from the iFactory and unlinking so that it can be opened and modified all on its own and is disconnected from the iFactory.

I am trying to send a bunch of iParts and some iAssemblies to somebody who doesn't want to work with an iFactory, and they are asking for everything to be independently modifiable.

[mcgyvr · Accepted solution]

I "think" so.. off the top of my head....

First open the factory ipart then do a save copy as.. Then open that copied one and delete all members but the one you want.. You should be prompted with a message that its not going to be an ipart anymore and you should be good to go..

[Anonymous]

Thank you for the quick response! Yes this works.... So I guess there isn't a more simple way to do this? Like a secret trick I am missing?

[johnsonshiue · Accepted solution]

Hi! Yes and no. iPart basically consists of an iPart factory ipt file and its iPart member ipt files. iPart member is basically a derive part of the factory computed from the row data. When you break the link between the iPart member file and the iPart factory, the iPart member will become a regular derive part. You can keep editing features but you won't be able to retrieve parent features from the factory.

To unlink the way you want it, you will need to open the iPart factory and activate the member row of interest. Save the factory as a different ipt file. Then delete the iPart table node from the newly saved part.

Many thanks!

[Anonymous]

Another question for you... All of my drawings reference is iFactory and then the Generated File. So the Model Reference has two files in it.

I try to replace the models with my new file I created from dumping the iFactory. It is the same part, just not an iPart

The drawing orphans all of the dimensions - is there any way to avoid this?

[Anonymous]

Thank you, this works, though in a brute force way. Do you know the answer to this question: 

All of my drawings reference an iFactory iPart and then the Generated File. So the Model Reference has two files in it.

I try to replace the models with my new file I created from dumping the iFactory. It is the same part, just not an iPart

The drawing orphans all of the dimensions - is there any way to avoid this?

[mcgyvr]

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@ejasperCAGPJ wrote:

Thank you, this works, though in a brute force way. Do you know the answer to this question: 

All of my drawings reference an iFactory iPart and then the Generated File. So the Model Reference has two files in it.

I try to replace the models with my new file I created from dumping the iFactory. It is the same part, just not an iPart

The drawing orphans all of the dimensions - is there any way to avoid this?

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Short of just leaving it an ipart then no there is typically no way of avoiding that..

The "internal references" to each edge/face,etc.. are different and thus Inventor does not know what is what anymore..

I'm not sure why you need to not have it be an ipart anymore but you might want to just leave it as an ipart

[Anonymous]

 Okay, so even though they are the same (the faces etc. are all the same) it orphans the dimensions.

The reason I have to separate this from the iFactory is because the person using this does not know what iFactory is and it doesn't follow their way of uploading files to the Vault (?). I am the only one that uses iFactory here and because it's different (and they have struggled with SolidWorks configs in the past) they are refusing to use it. So I have to separate out all of the files AND their drawings. The files now are not hard thanks to your solution. The drawings though... UGH!!! 

[mcgyvr]

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@ejasperCAGPJ wrote:

 Okay, so even though they are the same (the faces etc. are all the same) it orphans the dimensions.

The reason I have to separate this from the iFactory is because the person using this does not know what iFactory is and it doesn't follow their way of uploading files to the Vault (?). I am the only one that uses iFactory here and because it's different (and they have struggled with SolidWorks configs in the past) they are refusing to use it. So I have to separate out all of the files AND their drawings. The files now are not hard thanks to your solution. The drawings though... UGH!!! 

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Good luck.. 

My solution would be to simply train the other user to expand their knowledge and skill vs taking more time working around their current issues..

Please mark one of the posts above to "accept as solution" so this forum post can be considered closed.. 

Thanks

[johnsonshiue · Accepted solution]

Hi! The drawing dimensions and annotations become sick after you replace the iPart member file with the new part (iPart factory minus table). This is because the dimensions and annotations largely depend on the source document ID. The iPart factory would have a different document ID than the iPart member. So the sick dimensions are expected.

But, here is the workflow which should not lead to sick dimensions.

1) Create drawing views based on the iPart factory (active member).

2) Create dimensions and annotations on the views.

3) Exercise the de-table iPart workflow.

4) Replace model reference with the de-table parts.

Many thanks!

[Anonymous]

Thank you so much for this response!

Unfortunately, when I change the reference to be the Active Factory Member (and it is the right one) it orphans the dimensions still.

I tried what you said and many variations thereof but the dimensions still get sick. I think I'M gonna be sick now!

Thank you though so much for the quick and helpful responses!

[mcgyvr]

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@johnsonshiue wrote:

Hi! The drawing dimensions and annotations become sick after you replace the iPart member file with the new part (iPart factory minus table). This is because the dimensions and annotations largely depend on the source document ID. The iPart factory would have a different document ID than the iPart member. So the sick dimensions are expected.

But, here is the workflow which should not lead to sick dimensions.

1) Create drawing views based on the iPart factory (active member).

2) Create dimensions and annotations on the views.

3) Exercise the de-table iPart workflow.

4) Replace model reference with the de-table parts.

Many thanks!

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That did work on the simple part I did..

I wasn't sure if it would or not as many times the references are lost when I use replace model view like that in other situations.. This one just seems to work though..