Patten Curve Length

[douthett]

Inventor 2012

Is it possible to pattern a solid along a curved lenght inside a part?  So far I have not been able to but I can't figure out why I can't do it.

[JDMather]

Pattern a solid or pattern a feature?

Probably yes.

 http://home.pct.edu/~jmather/skillsusa%20university.pdf

Attach your file here.

[douthett]

I threw together a quick model of what I'm trying to do sicne I couldn't get the ok to send the real files.

[johnsonshiue]

Hi! If you want to pattern the whole solid along the path as multiple solid bodies, unfortunately it is not allowed. If you want to pattern the whole solid along the path as a feature, it can be done. But, the feature has to be patternable. Derive is not a patternable feature.

The closest workflow I can think of is to convert the Derive Assembly feature ot a patternable feature. Then pattern the feature along the path. Here is how you do it (please bear with me, since it is a bit awkward).

- Open test_Substitute_1.ipt

- Find a planar side face. Create a workplane exactly on top of it.

- Delete Face -> pick the planar face.

- Sculpt -> the deleted face body and the workplane. You will get the solid back.

- Rect Pattern -> pick the Sculpt feature -> pick the curve for Direction 1 -> set distance and number of instances -> expand the dialog >> set Orientation from Identical to Direction1 -> OK.

Let me know if it works for you.

Thanks!

[JDMather · Accepted solution]

Instead of deriving the assembly into a part could you create a path part and pattern workpoints on the path (make sure to set Direction 1).
Then place the path "part" into the assembly and use Pattern Component?

(see assembly in attached)

[ravikmb5]

use fusion to pattern a solid along a curve and bring back the model to the inventor environment

i follow this procedure

[douthett]

So you're saying Inventor can't do it and I need another program to do and then export it back to Inventor.  Is that correct?

[ravikmb5]

This a bug in inventor

We should wait for Next Release

http://forums.autodesk.com/t5/Autodesk-Inventor/INVENTOR-SP3-MULTI-BODY-Pattern/m-p/2676208#M373492

http://forums.autodesk.com/t5/Autodesk-Inventor/Pattern-solid-along-arc/m-p/2691707/highlight/true#M...

[alewer]

---

@ravikmb5 wrote:

We should wait for Next Release

---

Except that it was reported two releases ago (2010) and still hasn't been resolved (Case 05214239).  I wouldn't hold your breath.

[douthett]

I'm trying the method you suggested but for some reason when I place the file that has the Pattern Component in an assembly the Pattern Component disappears and I'm left with just the point.

Any ideas what I'm doing wrong?

[JDMather]

I'm not sure I follow.  The pattern component would be an assembly - therefore placing into another assembly would be a sub-assembly.

Attach the files where with the disappearing components.

[douthett]

The pattern doesn't show up in the tree so I can not select it. 

I've included the new dumbing files and the image of the tree

[douthett]

I found the solution for that problem.  I had it in Assembly View instead of Modeling View.  It works now