topic Re: Create a part in assembly with adaptive geometry in Inventor Forum

Create a part in assembly with adaptive geometry

danijel.radenkovic — Mon, 10 Apr 2017 09:20:05 GMT

Hello to all,

I have created a new part with referenced geometry to another part but I forgot the way how I did it sometimes in the past. Last few years I am working with multibody parts so I have forgot old way through assembly. Now, I am trying to do it again on the old way (through assembly), but as you can see on the attached video, geometry of the new part is not updated. Somehow projected lines are fixed-not adaptive. Where I am doing something wrong?

Any help is very appreciated.

Danijel

Re: Create a part in assembly with adaptive geometry

mdavis22569 — Mon, 10 Apr 2017 10:12:43 GMT

Look at 40 seconds into your video....

You make a rectangle.. that would need to be based on the adaptive. Also if you look at the line it's full of lock symbols

Re: Create a part in assembly with adaptive geometry

danijel.radenkovic — Mon, 10 Apr 2017 10:21:54 GMT

@mdavis22569 wrote:

Look at 40 seconds into your video....

You make a rectangle.. that would need to be based on the adaptive. Also if you look at the line it's full of lock symbols

Yes, I saw those fixed constraints but they are added automatically. Do I need to remove them manually and create a new collinear (or coincident) constraints?

Re: Create a part in assembly with adaptive geometry

Fouad-l — Mon, 10 Apr 2017 10:43:35 GMT

Hi.

Please tray to continue drawing the rectangle from the projected lines instead of using the rectangle command.

When you draw the rectangle, there is a line that overlies the adaptive line. I think the revolution operation uses the line of the new rectangle instead of the adaptive one.

Re: Create a part in assembly with adaptive geometry

mdavis22569 — Mon, 10 Apr 2017 10:43:52 GMT

working on a solution using adaptive (which I don't use often, and avoid at all cost)

Re: Create a part in assembly with adaptive geometry

danijel.radenkovic — Mon, 10 Apr 2017 11:29:31 GMT

@Fouad-l wrote:

Hi.

Please tray to continue drawing the rectangle from the projected lines instead of using the rectangle command.

When you draw the rectangle, there is a line that overlies the adaptive line. I think the revolution operation uses the line of the new rectangle instead of the adaptive one.

But I don't see the reason why it doesn't work? It has to be ok cause line of the rectangle is attached on the adaptive (projected) line and it is normal that rectangle's line ALWAYS move when adaptive line is moved. Am I right?

By the way, I have tried what you advised but attached geometry is still fixed. Actually, fixed constraints are added automatically and immediately after projecting the edges.

Re: Create a part in assembly with adaptive geometry

johnsonshiue — Mon, 10 Apr 2017 21:06:08 GMT

Hi Danijel,

The edges you were trying to project are silhouette edges. These edges are not actual edges. The geometry and topology of such edges can change based on the view direction and the sketch plane direction. Inventor never supports adaptivity on silhouette edges. You might have selected an actual edge to project before.

Many thanks!

Re: Create a part in assembly with adaptive geometry

danijel.radenkovic — Tue, 11 Apr 2017 09:09:08 GMT

@johnsonshiue wrote:

Hi Danijel,

The edges you were trying to project are silhouette edges. These edges are not actual edges. The geometry and topology of such edges can change based on the view direction and the sketch plane direction. Inventor never supports adaptivity on silhouette edges. You might have selected an actual edge to project before.

Many thanks!

Hello, Sir,

Thank you very much for the reply. So, I have used split face feature to get some visible edges. It works!

Perfect! Thank you very much!

Danijel