Can I make a flexible part in inventor?

[Anonymous]

Hi everybody

I have a question about Inventor

Can I make a flexible part in inventor?

Well, I have a kind of steel belt that around a tapered pole, then in inferior position this is placed in bigger diameter and the top this is placed in the smaller diameter but this have the same length Can we make an adaptive part that we can put in any diameters in the same assembly? And how we can do this?

I attach some pictures about this

[kgilham]

Albert,

It sounds like what you are looking for is positional reps for parts.  This is currently not possible in Inventor.  I have seen some companies append -01,-02 to the end of the part name in order to have the same part number.  

The development team is looking into adding this type of functionality in the future so if you are not already involved in our Beta forum you could sign up to receive more information about what the team is considering and give us feedback on what we can do to improve this area of Inventor.

[Fouad-l]

Hi @Anonymous.

If you know exactly the diameter values, you can create an iPart with these values and insert them in an iAssembly, then you will have all parts you need controled by a parameter you choose. You can then (if needed) create ipart's elements as individual parts and give them a name.

[Fouad-l · Accepted solution]

This is a screencast of what i mean.

http://autode.sk/2rhFmS8

To keep same length you can use math rules inside parameters such as :

[TheCADWhisperer]

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@Anonymous wrote:

Well, I have a kind of steel belt ...

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Can you attach the ipt part of this steel belt here?

[mcgyvr]

From what I see in the images thats a perfect job for iparts/iassemblies..

The steel band would be an ipart and an iassembly created with all the different diameters needed..

Custom parameter column to have unlimited sizes as needed..

You could just do it all as an ipart and avoid the iassembly too if you wanted..

[Anonymous]

Ok thanks 

I understand that now there is no tool to make a flexible part. But I can use an iPart making many files but with the same part number.

and How can I join to the Beta Forum???

[Anonymous]

Ok thanks!

I going to try make an iPart to solve this conflict. 

at this time just one time I tried the iassembly in a class is some complicated

But I going to review this topic

Thanks you very much for your Help and time

[Anonymous]

Now I don't made this model yet

but when I have it, I share it

Thanks you very much

[TheCADWhisperer · Accepted solution]

I would create a named parameter Total_Length.

You will have an Arc radius dimension.  I would make this a named parameter

I would then add a driven Arc_Length dimension.

Then I would add 2*straight length dimension (Total_Length-Arc_Length).

In your iPart you can set a range of dimension for the Arc radius or Discrete values.

All of the other dimensions will automatically update to maintain the constant Total_Length value.

[sepehr.ariaei]

Is this still not possible in Inventor 2019? @kgilham 

[TheCADWhisperer]

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@sepehr.ariaei wrote:

Is this still not possible in Inventor 2019? @kgilham 

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Attach your *.ipt file here.

[johnsonshiue]

Hi! Indeed, Inventor is not yet able to create a flexible part. A part which has variable definitions like a rod varying in length depending where it is used. We are aware of the deficiency and we are investigating the solution.

In the meantime, you can achieve similar behaviors by using adaptive parts and copy of adaptive parts. Regardless, you cannot have one single ipt file representing multiple definitions at the moment.

Many thanks!

[RyanRausch]

Has anything been in development for creating flexible parts within an Inventor part?

[johnsonshiue]

Hi Ryan,

No, the so-called flexible part isn't supported yet. Are you talking about the ability to have infinite variation of a given part body? Or, you want to have multiple variations, controlled by a table? If it is latter, it is available in Model States (2022 and later releases).

Many thanks!

[JDMather]

@RyanRausch 

Can you Attach your *.ipt file here?

[RyanRausch]

@JDMather 

 Attached is the part file.  This is a purchase part that is a trolley for a flat cable festoon system.  The only parameter that we would want to be flexible is called THICKNESS which would range anywhere from 0" to 1".

Let me know if you have additional questions. 

[RyanRausch]

@johnsonshiue 

Attached is the part file.  This is a purchase part that we use that is a trolley for a flat cable festoon system.  The parameter I would like to be able to be "flexible" is THICKNESS.  We would like it to be flexible in order not to have to save multiple variations of the same part for infinite thicknesses of flat cable.  

[johnsonshiue]

Hi Ryan,

The closest thing in Inventor to accommodate that is to create custom iPart. In your case, you can convert the part to an iPart and make Thickness a custom column. When placing the part to an assembly, you will be prompted to enter the Thickness value. The other way is to use Place iLogic Component command and you may enter the desirable Thickness value on placement. Regardless of either approach, you will need to create multiple files. Each file has a unique value of Thickness.

Many thanks!

[JDMather]

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@RyanRausch wrote:

The only parameter that we would want to be flexible is called THICKNESS which would range anywhere from 0" to 1".

Let me know if you have additional questions. 

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The problem with not defining this with different part numbers is that a change is a change everywhere.