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Extract iPart from Content Center Library?

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Message 1 of 14
bruce.buck
2559 Views, 13 Replies

Extract iPart from Content Center Library?

Is this even possible? Found a part in a generic library that we could use in our custom library. However, I need to make a few tweaks with the geometry and other parameters like adding our custom material styles to it. Is there a way to get the original iPart from the library?

Inventor 2015 SP1 Build 203 Update 3
Vault Professional 2015 Build 19.1.13.0 Update 1
AutoCAD 2015 SP2 J.210.0.1
NavisWorks Manage 2015 SP3 12.3.0.115750
PLM360
13 REPLIES 13
Message 2 of 14
mdavis22569
in reply to: bruce.buck

You could File save copy as .... and go from there or redraw it from scratch

Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.

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Mike Davis

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Message 3 of 14
LT.Rusty
in reply to: bruce.buck

No problem at all to do this.

 

Capture.JPG

Rusty

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Message 4 of 14
cbenner
in reply to: bruce.buck

Material and other properties can be added to the family table itself once you have copied it to your custom library.  (use save copy as).

 

Geometry changes can be made by opening one member of the part from the CC, using "as custom".  Make your changes and save the custom part.  Go back to the CC and right click the family and select Replace Family Template.  Then find and select the part you just modified.  Now... caveat.... depending on how extreme your changes are it might be easier just to recreate the ipart from scratch.  If you are adding tabulated dimensions, for example, I'm not sure how it will behave.  If you make note of the added parameters, you may be able to just add those manually to the family table and hand enter the values.  I've never done this, so proceed with caution.  Simple geometry changes work well with the Replace Family Template.

 

Try it, if you "save copy as", you've got nothing to lose but time.  You can always delete the family if it fails, and try again.

Message 5 of 14
bruce.buck
in reply to: mdavis22569


@michaeldavis7418 wrote:
You could File save copy as .... and go from there or redraw it from scratch

When I choose that from the library, I don't have an option to save it any other place than another library (see screenshot). 4-17-2014 12-00-17 PM.jpg

Inventor 2015 SP1 Build 203 Update 3
Vault Professional 2015 Build 19.1.13.0 Update 1
AutoCAD 2015 SP2 J.210.0.1
NavisWorks Manage 2015 SP3 12.3.0.115750
PLM360
Message 6 of 14
bruce.buck
in reply to: LT.Rusty


@LT.Rusty wrote:

No problem at all to do this.

 

Capture.JPG


 

When I do that, I don't get the family table, just that individual member.

4-17-2014 12-04-39 PM.jpg

Inventor 2015 SP1 Build 203 Update 3
Vault Professional 2015 Build 19.1.13.0 Update 1
AutoCAD 2015 SP2 J.210.0.1
NavisWorks Manage 2015 SP3 12.3.0.115750
PLM360
Message 7 of 14
LT.Rusty
in reply to: bruce.buck

Ah, okay, I see what you're trying to do.

 

For some reason I thought you just wanted to extract a part, and missed that you wanted to tweak the whole family.

 

 

Okay, to start with, have you created a Read/Write library in your project file?  If not, close all open files and click on PROJECTS on the GET STARTED tab.  Right above the DONE button there's a pull-down with only one button on it.  Go there, and find the options to create a read/write library.

 

Once you have your library created, go to the Content Center Editor on the MANAGE tab.  (Hint: you have to have a file open to do this, so I usually just create a new assembly.)  Change the LIBRARY VIEW pull-down to show whatever library your generic part is in, then browse to the type of part you want.  All of the families and categories are ghosted out, becuse they're Read Only.  Right click on the one you want to duplicate, then pick COPY TO and your new Read/Write library.

 

Once the copy process is complete, change the LIBRARY VIEW pull-down to go to your Read/Write library.  Once you're there, right click on your new family, and you'll have a bunch of new options.  FAMILY TABLE will let you edit the iPart table.  FAMILY PROPERTIES will let you rename your family.  REPLACE FAMILY TEMPLATE will let you replace the part template that is used to create your part.  (Use this, for instance, if you want to change the geometry, or if there's other parameters that you need to have available in the table that aren't already there.) 

 

 

 

 

 

Rusty

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Message 8 of 14
bruce.buck
in reply to: cbenner


@cbenner wrote:

Material and other properties can be added to the family table itself once you have copied it to your custom library.  (use save copy as).

 

Geometry changes can be made by opening one member of the part from the CC, using "as custom".  Make your changes and save the custom part.  Go back to the CC and right click the family and select Replace Family Template.  Then find and select the part you just modified.  Now... caveat.... depending on how extreme your changes are it might be easier just to recreate the ipart from scratch.  If you are adding tabulated dimensions, for example, I'm not sure how it will behave.  If you make note of the added parameters, you may be able to just add those manually to the family table and hand enter the values.  I've never done this, so proceed with caution.  Simple geometry changes work well with the Replace Family Template.

 

Try it, if you "save copy as", you've got nothing to lose but time.  You can always delete the family if it fails, and try again.


Ok, so if I understand you correctly, you can't get the original ipart, but can modify an "as custom" family member and replace to propogate changes.

 

Regarding the Materials, do you do that through the "Material Guide function"?

4-17-2014 12-16-13 PM.jpg

 

What I'm trying to do on this particular one is add a Material that is part of our custom material library. Clicking on the list only has the Materials that were part of the original iPart:

4-17-2014 12-19-36 PM.jpg

Inventor 2015 SP1 Build 203 Update 3
Vault Professional 2015 Build 19.1.13.0 Update 1
AutoCAD 2015 SP2 J.210.0.1
NavisWorks Manage 2015 SP3 12.3.0.115750
PLM360
Message 9 of 14
cbenner
in reply to: bruce.buck

Material guide is not what you want, that will give you a wizard to help you create a copy of a family to a new material.  For example, you have this part in Stainless, you can copy the family exactly as is to Titanium.

 

Not sure if you can pick a custom material from the list, or change what list that pulls from.  I don't do anyhting with custom materials, so I fear I have no answer to that one.

Message 10 of 14
cadman777
in reply to: bruce.buck

Bruce,

 

Sorry for the late reply. I was forraging thru this forum to find the answer to a CC question, which is posted by Chris Benner in here (Thanx Chris!).

 

You have to create your own material in the "Styles and Standards Editor", and make it available in your materials library.


Here's how I create the new material:

Open the Styles Editor, expand the "Materials" category in the left dialogue window.

Scroll down till you find a material that's similar to your custom material, and edit all the properties to suit your new material.

 

For example:

 

"Stainless Steel, 316L" is not in the out-of-the-box list, so I RMB on "Stainless Steel 316", and select "New Style".

Then I go into that new style and check the properties.

Since all the properties shown for 316 are identical to 316L, I just close-out that dialoge and have my new material.

 

Next, you have to make your new style available to all your parts, so you have to do this procedure:

 

Close all your files, and open the Project dialogue.

In there, you see in the bottom window "Use Style Library = Read Only" (the default option).

RMB on that text and select "Yes".

Then "Save" at the bottom of the dialogue box.

 

Now re-open your assembly, and start the BOM for that assembly, and change all the parts that need your updated material.

 

That's my work-flow.

 

Hope this helps, even though it's very late ...

... Chris
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Message 11 of 14
cad
Advocate
in reply to: LT.Rusty

It will make the stuff far quicker for me to edit my published library.

But I'm getting an error message as attached while trying to use "Replace Family Template" in CC Editor.

 

Can I get any solution where am I going wrong?

Thanks.

Message 12 of 14
Mark.Lancaster
in reply to: cad

@cad

 

Usually that means the information that you are using to replace the family template doesn't really match what was there before.  Without know what your family template was originally configured as and what you changed, there's no way in telling you what needs to be corrected.

Mark Lancaster


  &  Autodesk Services MarketPlace Provider


Autodesk Inventor Certified Professional & not an Autodesk Employee


Likes is much appreciated if the information I have shared is helpful to you and/or others


Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.

Message 13 of 14
cad
Advocate
in reply to: Mark.Lancaster

I tried out as below, just to recognize a trouble.

 

1. I made an iPART.

2. I published it to CC

3. Copied iPART to sub folder.

4. Added one more row to table and saved. (I didn't changed anything else)

5. Tried to REPLACE, previously published in CC with new iPART.

6. Got an error.

Message 14 of 14
Mark.Lancaster
in reply to: cad

@cad

 

That's not a proper workflow..  Replace family template means..

 

1.  You place that CC component into an assembly as a custom content center or your opened from content center, selected your component and the option to open as a custom part.

2.  You saved your custom CC.

3.  You modified that instance

4.  You go back into CC Editor and perform the replace family table.

 

In your case, if you want to add another row, go into CC Editor and edit the family table and add the row.

 

Once a component is published to the CC you no longer need the ipart file that you created.  But I was always recommend to keep them around just in case you have to start something from scratch.

Mark Lancaster


  &  Autodesk Services MarketPlace Provider


Autodesk Inventor Certified Professional & not an Autodesk Employee


Likes is much appreciated if the information I have shared is helpful to you and/or others


Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.

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