Inventor General Discussion

Inventor General Discussion

Reply
Mentor
MikahB
Posts: 208
Registered: ‎10-11-2009
Message 1 of 5 (400 Views)

Break Link En Masse After Make Components

400 Views, 4 Replies
06-27-2012 10:58 AM

I got a STEP file from a client that contains about 260 individual bodies.  The file imported okay as a single IPT, then I used Make Components to create an assembly of individual parts.  Now, I've got 260 parts that all are linked to the original file, and I can't find a way other than part-by-part editing to break the links.

 

Is there another import process I should use to avoid this, or is there some way I'm not aware of to Break Links without doing it part-by-part?

Mikah Barnett
All Angles Design
Product Design Suite Ultimate 2014
Windows 7 Professional x64
Intel i7-3770k @ 4.5GHz
32GB DDR3-2400 RAM
GeForce GTX 670 4GB
Distinguished Mentor
rdyson
Posts: 918
Registered: ‎04-11-2005
Message 2 of 5 (394 Views)

Re: Break Link En Masse After Make Components

06-27-2012 12:37 PM in reply to: MikahB

I'm guessing that you had "Import as single part" checked. Unchecked, an assembly step will import as an assembly. 

 

SNAG-0000.png

Mentor
MikahB
Posts: 208
Registered: ‎10-11-2009
Message 3 of 5 (385 Views)

Re: Break Link En Masse After Make Components

06-27-2012 01:22 PM in reply to: rdyson

Nope, I did not have that option checked.  Here is my options screen at import time - this results in a multi-body part with lots of bodies.

 

 

Mikah Barnett
All Angles Design
Product Design Suite Ultimate 2014
Windows 7 Professional x64
Intel i7-3770k @ 4.5GHz
32GB DDR3-2400 RAM
GeForce GTX 670 4GB
Product Support
bobvdd
Posts: 577
Registered: ‎11-23-2005
Message 4 of 5 (357 Views)

Re: Break Link En Masse After Make Components

07-02-2012 02:22 PM in reply to: MikahB

Weird.

Anyway, looks like the damage is already done as you now have 260 files linked to the same parent.

A relatively easy way of breaking the derived link in multiple files is to use the CodeInjector tool that I have posted on the Inventor support blog

And "inject" below piece of iLogic code. The tool allows you to delete the rule after it has been run, and that is probably what you want to do to not "pollute" the ipt files..

 

Cheers

Bob

 

Dim rcomp As Inventor.ReferenceComponent
Dim refcomp As Inventor.Document
refcomp = ThisApplication.ActiveDocument
If refcomp.ComponentDefinition.ReferenceComponents.DerivedPartComponents.Count > 0 _
And refcomp.ComponentDefinition.IsiPartMember = False Then
For Each rcomp In refcomp.ComponentDefinition.ReferenceComponents.DerivedPartComponents
If rcomp.Type = Inventor.ObjectTypeEnum.kDerivedPartComponentObject And rcomp.LinkedToFile Then
rcomp.BreakLinkToFile
refcomp.Save
End If
Next rcomp
End If
If refcomp.ComponentDefinition.ReferenceComponents.DerivedAssemblyComponents.Count > 0 _
And refcomp.ComponentDefinition.IsiPartMember = False Then
For Each rcomp In refcomp.ComponentDefinition.ReferenceComponents.DerivedAssemblyComponents
If rcomp.Type = Inventor.ObjectTypeEnum.kDerivedAssemblyComponentObject And rcomp.LinkedToFile Then
rcomp.BreakLinkToFile
refcomp.Save
End If
Next rcomp
End If

 

Mentor
MikahB
Posts: 208
Registered: ‎10-11-2009
Message 5 of 5 (332 Views)

Re: Break Link En Masse After Make Components

07-03-2012 09:03 AM in reply to: bobvdd

Thanks, Bob - that does seem like a workable solution.  I have just been unlinkning manually as I use individual parts.  Still a pain in the butt, but at least it's less pain spread out over several days!

 

I will try your solution in the next couple weeks on a smaller import and see if I can make it go!

Mikah Barnett
All Angles Design
Product Design Suite Ultimate 2014
Windows 7 Professional x64
Intel i7-3770k @ 4.5GHz
32GB DDR3-2400 RAM
GeForce GTX 670 4GB
Post to the Community

Have questions about Autodesk products? Ask the community.

New Post
Announcements
Do you have 60 seconds to spare? The Autodesk Community Team is revamping our site ranking system and we want your feedback! Please click here to launch the 5 question survey. As always your input is greatly appreciated.