Adapting Part Size to Other Parts in Assembly

[Anonymous]

Hi , 

I am having difficulty figuring out how to make one part in my assembly (simple angle extrusion) match the same height as another part in my assembly. This has been very simple for me to do in the "Part" environment in the past but now that I am in the assembly environment, I am unable to use parts parameters in my equations. 

Here is a picture of what im trying to do.

The height of this plate will change all of the time and I need the height of the angle to also change with it. In the picture the angle height does not reach the top although it is supposed to no matter what height I choose for the plate. 

Any help is greatly appreciated!

Thanks

Sandro

[Jonathan.Landeros]

Can you link them mathmatically using parameters? 

http://www.inventortales.com/2013/04/linking-parameters-from-one-part-to.html

[Anonymous]

Jon,

There may be a way but I am slightly inexperienced with Inventor. I have tried using the parameters but it does not seem to work. There are "Assembly Parameters" and "Part Parameters."

While in the assembly environment I can not link one parts parameters to anothers. There may be a way but I do not know how to do it.

[JDMather]

Can you attach your assembly here?

[Jonathan.Landeros · Accepted solution]

The video in the link should show it, although I created it a long time ago, so I don't *exactly* recall what's in there.

I would link the part parameters to the part parameters.  In other words you would import the required dimensions from the plate into the angle. Then when your editing the angle, build equations that get what you want. 

Breaking down the steps as best I can. 

1) Rename the parameters you need to link in the plate.  "Plate_Length" is easier to deal with than "d3"

2) Open the Angle part.  Use the Derive Component tool (On manage tab) to import the parameters from the plate

3) Edit the dimensions features and sketches and build the appropriate dimensions inside the angle.

For example take the dimension defining the lenght of the angle and type "=Plate_Length/4".  This makes the length of your angle a quarter of the length of the plate.

I hope this helps.  Remember, when renaming paraemeters don't use spaces, use underscores ("Part_Length" not "Part Length").  Inventor errors out on spaces in the parameter screen.

[johnsonshiue]

Hi! This one looks like an ideal candidate for adaptive modeling. Does the relationship only exist within this particular assembly? I assume it is. Here is what you need to do to establish adaptive relationship.

1) Change the browser view from Assembly View to Model View.

2) Find the Extrusion feature needed to be adaptive.

3) Right-click on the Extrusion -> check Adaptive.

4) Create assembly constraints on the side faces so the Extrusion will adapt.

There is one catch though. The sketch consumed by the Extrusion needs to be as free as possible. If you have certain dimensions, make sure they don't violate the adaptive behavior. Otherwise, adaptivity will fail.

Let me know if it works for you.

Thanks!

[Anonymous]

Jon, This worked perfectly. I have no Idea I could simply import parameters that actually adapted to my changes. This is fantastic.

I have no idea what was going wrong with the adaptability features (other than I've never used them), but the end result of this is exactly what I was looking for.

Thanks!
Sandro

[JDMather]

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@Anonymous wrote:
I have no idea what was going wrong with the adaptability features ...

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Which is a very good reason for attaching assembly here.