Inventor General Discussion

Inventor General Discussion

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shuaib_cad
Posts: 47
Registered: ‎11-09-2011
Message 1 of 12 (860 Views)
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Is there flexible part option in assembly?

860 Views, 11 Replies
12-07-2012 09:14 AM

Is there flexible part option in assembly?

 

I have a shaft for which i want to vary my diameter in the assembly without affecting the part.

Is it possible in Inventor?

Its there in ProE. Its called "Flexible".

Hi shuaib_cad,

 

As others have mentioned the functionality you're asking for can be found by making an iPart, and then creating a custom column or custom cell input as shown in the illustration below. Once a column or cell has been designated as a custom parameter, you can specify a range or increment (if needed). When placed in an assembly you are prompted to enter a size of your choosing at that time.

 

How to create a custom iPart (taken from the help files):

 

  1. Create a standard iPart.
  2. On one or more tabs in the iPart Author, determine the custom values to enter when the iPart is placed.
  3. If the value is not already in the iPart table, select it in the left pane, and then click the Include arrow to add it.
  4. In the iPart table, specify cells or columns in which to enter a custom value:
    • Right-click in a column and select Custom Parameter Column.
    • Right-click in any cell and select Custom Parameter Cell. Use this technique to create only one row that allows custom entry.

    A custom column or cell is indicated by a blue background.

  5. Save the file.

 

Autodesk Inventor Custom Ipart Column.png

 

 

For more reading on custom iParts see the How do standard and custom iParts differ? topic at this link:

http://wikihelp.autodesk.com/Inventor/enu/2013/Help/1310-Autodesk1310/1500-Parts1500/1580-iFeature1580/1586-iPart_Fu1586

 

Other options would be to use iLogic to set the part up, or publish the iPart to Content Center and use it as a content center component.

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

*Expert Elite*
karthur1
Posts: 4,264
Registered: ‎04-27-2005
Message 2 of 12 (856 Views)

Re: Is there flexible part option in assembly?

12-07-2012 09:37 AM in reply to: shuaib_cad

I think you are looking for "adaptive" in Inventor.

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blair
Posts: 4,229
Registered: ‎11-13-2006
Message 3 of 12 (838 Views)

Re: Is there flexible part option in assembly?

12-07-2012 11:39 AM in reply to: shuaib_cad

Flexible is used for sub-assemblies within assemblies. Having a cylinder assembly that you want to stroke within assembly.

 

An adaptive part changes with repect to geometry referenced by another part within the assembly. If the shaft diameter is adaptive (projected geometry from a bore-hole), when the bore hole changes the diameter of the shaft will change.

 

If you want parts to change by tables, you might look at iParts.

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shuaib_cad
Posts: 47
Registered: ‎11-09-2011
Message 4 of 12 (797 Views)

Re: Is there flexible part option in assembly?

12-09-2012 06:49 PM in reply to: blair

@ above...

 

I dont want to use iparts. What i want is, as soon as i place a shaft in assembly mode it should ask for the diameter of the shaft in a dialog box. I should be allowed to change the diameter of the shaft without affecting the part.

For example: when we place a bolt from content center, it asks for the diameter in a seperate dialog box.

Is it possible?

 

If yes, then please upload the file.

*Pro
sbixler
Posts: 1,934
Registered: ‎09-15-2003
Message 5 of 12 (778 Views)

Re: Is there flexible part option in assembly?

12-10-2012 04:32 AM in reply to: shuaib_cad

shuaib_cad wrote:

... I should be allowed to change the diameter of the shaft without affecting the part.


In Inventor this makes no sense.  The part is the shaft.  Even with your example of a bolt from the Content Library, you make the selection, then the part gets created to that dimension.

 

If it is specifically a shaft that you want, you might look at the Design Accelerator for shafts.  Or, you can create your own Content Library shaft that will allow you to choose dimension(s) before placement.  But you can't change a component of an assembly without changing the model, because that's all the component is.

*Expert Elite*
jclaidler
Posts: 547
Registered: ‎10-29-2009
Message 6 of 12 (775 Views)

Re: Is there flexible part option in assembly?

12-10-2012 04:48 AM in reply to: shuaib_cad

What you are asking about, is an iPart.

John Laidler


AutoCAD 2014 | Inventor Professional 2014 | Navisworks Manage 2014 | Vault Professional 2014
Active Contributor
shuaib_cad
Posts: 47
Registered: ‎11-09-2011
Message 7 of 12 (753 Views)

Re: Is there flexible part option in assembly?

12-10-2012 10:43 PM in reply to: jclaidler

@ above...

I am well aware about iparts.... but what i am asking is something else....

 

shaft was just an example.... what i want is as soon as i place a part it should ask for some specified dimensions of the part... when i give those inputs the part should be placed... but the orginal ipt should not change its dimensions... 

 

its called flexible part dimension in ProE assembly.... i thinks its not possible in inventor....

 

coming to iparts... i have to create multiple parts in the ipt (which means if i want my diameter to vary between 50-100, then i have to insert 50 rows which in turn creates 50 ipt files).

 

If we have flexible part option to vary the part dimensions in assembly (like for content center) it would be easier and file size will be reduced.

 

If you know how to create such parts like conent center parts, please upload the file. it would be very useful for me.

 

*Pro
sbixler
Posts: 1,934
Registered: ‎09-15-2003
Message 8 of 12 (747 Views)

Re: Is there flexible part option in assembly?

12-11-2012 04:05 AM in reply to: shuaib_cad

You can certainly create your own Content Library parts.  You want to place as Custom, which allows specifying a dimension or dimensions rather than picking them from a table.  I don't have any instructional materials, and I haven't done such a thing for a year or two, so someone else will have to jump in here.  If you search in the Help and in this forum, I think you should search on Publish to Content Center (or Library), and also Part Authoring.

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harco
Posts: 879
Registered: ‎02-16-2006
Message 9 of 12 (738 Views)

Re: Is there flexible part option in assembly?

12-11-2012 04:30 AM in reply to: shuaib_cad

Create a new assembly and try placing the attached ipart.

Browse to save new file.

Set your dims.

Click in the window.

Dismiss.

 

Does this do what you want?

Valued Contributor
nannerdw
Posts: 95
Registered: ‎06-09-2008
Message 10 of 12 (719 Views)

Re: Is there flexible part option in assembly?

12-11-2012 08:27 AM in reply to: shuaib_cad
shuaib_cad wrote: coming to iparts... i have to create multiple parts in the ipt (which means if i want my diameter to vary between 50-100, then i have to insert 50 rows which in turn creates 50 ipt files).

If we have flexible part option to vary the part dimensions in assembly (like for content center) it would be easier and file size will be reduced.


Those 50 parts are still derived from a single base part.  Any changes you make to the base part will be reflected in all of its derived iParts.

 

Also, Content Center parts are iParts.  Each time you place a component from the content center or change its size, Inventor checks to see if the iPart with the specified dimensions has already been created, and if not, it creates a new iPart file.

-Using Autodesk Inventor Professional 2012
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