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".
Solved! Go to Solution.
Solved by Curtis_Waguespack. Go to Solution.
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.
@ 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.
@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.
@ 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.
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.
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?
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.
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):
A custom column or cell is indicated by a blue background.
For more reading on custom iParts see the How do standard and custom iParts differ? topic at this link:
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
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.
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!
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!
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