Spring travel between Positional Configurations

[ztdservices]

Hi 

I have an assembly that contains a spring that moves flexibly within a fixed offset. I have now created 3 positional configurations within the assembly so I can show the specific state of the tool in certain conditions. However, when I move between the positions I cannot get the spring to update its length within the assembly. 

Any ideas on how to get round this?

Kind Regards

Jason

[swalton]

I don' think that Inventor will do what you want out of the box.  You will have to trick it.

I can think of two different approaches.

1. Make 3 different springs, possibly an ipart, and use assembly design views to show/hide each spring model depending on the position rep.

2. Use iLogic to control the length of the spring.  Tie a parameter in the assembly and the spring part to the position rep so that the spring changes size with the position reps.  I don't know enough iLogic to know if this will work the way I want it to.

For a one-time thing, I'd just use option 1 and move on.

[CCarreiras]

Hi!

Try hit the button "Rebuild All" after you change the positional rep.

[jtylerbc]

If you need to be able to show the spring correctly in a drawing at multiple positions, @swalton's first suggestion is really the only thing that works. 

Intelligence can be built into the part so that it can adjust its length relative to other parts in the assembly.  There are several ways to do this (iLogic, VBA, Adaptivity).  However, the part can still only be one length at a time.  There is currently no way in Inventor to build a truly Flexible part that can exist in multiple states at the same time.

[MechMachineMan]

To make a single ipt change length within the context of an assembly you have 3 options:

1) Adaptavity on the part

2) iLogic

3) Linked parameters

To give it the appearance of changing you have another option; although none work fluidly with just positional reps.

- Have 3 different spring models. Tweak visibility of the springs on/off as required to show the proper spring length.

Good luck.

[kelly.young]

Hello @ztdservices the previous replies provide some good insight. I made this screencast a little while back, should help you with your problem.

Please select the Accept as Solution button if a post solves your issue or answers your question.

[johnsonshiue · Accepted solution]

Hi Guys,

I think Steve is right. Currently, Inventor part (the spring) can only be represented in one geometric definition in one part file. If you need to have multiple geometric definitions, you will need to make them different parts. Adaptivity does not overcome the limitation. It only makes the part changed by the influence of assembly constraints. But, it does not change the fact that one geometric definition in one part.

We are aware of the limitation and we are working on a solution to make it better.

Many thanks!