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Is there flexible part option in assembly?

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Message 1 of 16
shuaib_cad
3295 Views, 15 Replies

Is there flexible part option in assembly?

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".

15 REPLIES 15
Message 2 of 16
karthur1
in reply to: shuaib_cad

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

Message 3 of 16
blair
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.


Inventor 2020, In-Cad, Simulation Mechanical

Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
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Message 4 of 16
shuaib_cad
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.

Message 5 of 16
SBix26
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.

Message 6 of 16
john.laidler
in reply to: shuaib_cad

What you are asking about, is an iPart.

John Laidler
AutoCAD, Inventor and Vault



Please use "Accept as Solution" & give "Kudos" if this response helped you.
Message 7 of 16
shuaib_cad
in reply to: john.laidler

@ 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.

 

Message 8 of 16
SBix26
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.

Message 9 of 16
harco
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?

Message 10 of 16
nannerdw
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.

Message 11 of 16

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-iFeature15...

 

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

Message 12 of 16

@Curtis_Waguespack 

Thanks a lot...!!!!

This is the only solution for this issue....Smiley Happy

Message 13 of 16
CMyers
in reply to: shuaib_cad

I am totally with you on this.  I am a long-time Pro/E (Creo) user, and it's really frustrating to not have flexible parts in Inventor.  Flexible parts allow you to have things like springs without creating a bunch of discrete parts showing each possible position (length) of a spring.  A flexible part would be similar to flexible assembly, where it would be a different "representation" (for lack of a better word) of a possible state of an object.  My specific example has to do with having a belt with flexible length as an flexible assembly is adjusted.  I would settle for an assembly surface to represent the belt, but that doesn't exist either!  I don't know why CUT has to be the ONLY possible option for creating an extrusion in an assembly, and I don't know why we can't have a part be flexible and not have to create extensive, unwieldy iParts and iAssemblies to achieve what is possible in other CAD software.

Message 14 of 16
johnsonshiue
in reply to: CMyers

Hi! Indeed, this is something Inventor currently is lacking. Each component (part or assembly) needs to have a unique definition at any given moment. It cannot have more than one geometric definition. iPart and iAssembly are for different purposes. They are best for library content when definitions are similar but they need to be different part numbers. iPart and iAssembly are not a solution for flexible part. We are aware of the requirement. We are investigating good solution benefiting a lot of users.

Many thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 15 of 16
CMyers
in reply to: CMyers

Hi, and thank you for responding! I appreciate you taking the time to reply to my message. I appreciate that in general a part or assembly would have one geometric definition, but there are cases where that is not necessarily true (such as assemblies where adjustability is a key feature, or a spring that has one defining geometry but can be used in a multitude of places, or an o-ring or belt that needs to stretch to meet the specific application). This kind of adjustability is likely why flexibility for assemblies was made possible, and I would truly love to have that capability for components such as springs, belts, o-rings, etc to be able to make effective use of the assembly flexibility. The power of flexibility is that the basic definition of the assembly doesn't change with each use within different assemblies, which would mean we'd only need one defined assembly (or hopefully someday a part) that we could put in the Library and use as needed.

iParts and iAssemblies are great unless you have basically an infinite number of possible solutions, and Vault doesn't always play nice with them. In our case we have adjustable frame lengths and corresponding belt lengths for conveyors, plus left hand vs right hand arrangements. Users must select the frame length and corresponding belt length for each conveyor segment assembly in each system. We have 3 sets of iParts or iAssemblies per conveyor segment in 1/8" increments for each, and a lot of time was spent defining these so that we can swap them out as required for the system design. We have ended up with a huge number of iParts and iAssemblies for every possible scenario to the nearest 1/8" (frames, belts, segment assemblies, left, right, color, etc). People have copied the designs for different types or length ranges, which balloons the number of Vault items to maintain and increases the potential for things to get messed up.

What I would love to be able to do is place the defining conveyor segments where they need to be for the system space constraints, add the intermediate segment and constrain it such that it fills the gap between those defining segments. The nice thing about flexible assemblies is that we can have a different length of the adjustable length segment for the different gaps between segments, but only have one part number per frame, belt, and segment assembly. I was able to create the flexible assembly with the necessary adjustability, but have been unable to find a solution for the belt that would not end up creating a new part number for each use within the system assembly. I would be able to accept a solution where a surface (driven by an assembly sketch) could be used to represent the belt, but I can't put a surface in place that wouldn't cut the assembly. So close, and yet so far!!

P.S. An additional item of interest is to be able to have a perimeter dimension option for closed sketches, where the user would be able to select one dimension to vary that would maintain the desired perimeter, or even use a reference perimeter dimension to calculate the amount of belt length needed for a system.


Hi! Indeed, this is something Inventor currently is lacking. Each component (part or assembly) needs to have a unique definition at any given moment. It cannot have more than one geometric definition. iPart and iAssembly are for different purposes. They are best for library content when definitions are similar but they need to be different part numbers. iPart and iAssembly are not a solution for flexible part. We are aware of the requirement. We are investigating good solution benefiting a lot of users.

Many thanks!


Carolyn Myers
Sr. Mechanical Engineer

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Tech Logic Corporation
835 Hale Avenue N
Oakdale, MN 55128
Dir: 651-389-4903
Off: 651-747-0492
TF: 800-494-9330
cmyers@tech-logic.com
www.tech-logic.com

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Message 16 of 16
johnsonshiue
in reply to: CMyers

Hi Carolyn,

 

Regarding the dimension, I guess you want a loop dimension, right? Indeed, currently you would have to sum up each segment in the loop to do that. Technically and mathematically, it should be doable but it can be tricky to implement. We would need to watch out for generated segments (arc or line shrinking to a point). Anyway, this is a good suggestion. Please feel free to post it on Inventor Ideas if there isn't an existing one.

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer

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