topic A bug in update 3 of Inventor 2019 ? in Inventor Forum

A bug in update 3 of Inventor 2019 ?

liminma8458 — Mon, 18 Mar 2019 13:12:14 GMT

We just have to uninstall update 3 for Inventor 2019 and go back to the original release of Inventor 2019. The update 3 makes wrong area calculation at least in a shrinkwrap part. We normally create shrinkwrap part from a metal assembly to calculate its shot blasting area.

Attached is a demo assembly of 3 stacking cubes (cube with 1 inch edge). The area for the resulted shrinkwrap part should be 16 inch sq. But the update 3 calculation shows 18 inch sq. as below picture. Looks it still includes the overlapped areas. This behavior will accumulate for a big assembly and results in big wrong number.

There is not such problem in the original release of Inventor 2019.

Is it a bug for the update 3? how can we fix it ?

Thanks

Re: A bug in update 3 of Inventor 2019 ?

johnsonshiue — Mon, 18 Mar 2019 21:27:00 GMT

Hi! Actually, the change in behavior is a fix to address inconsistency in physical properties between shrinkwrap part and the source assembly. Shrinkwrap part is a simplified form of the source assembly. The properties should be identical to the source. If you want to have a merged body part, you should use Derive Assembly command so that the physical properties are evaluated based on the derived geometry. Please install 2019.3 update back.

Many thanks!

Re: A bug in update 3 of Inventor 2019 ?

liminma8458 — Mon, 18 Mar 2019 23:37:45 GMT

Where is the Derive Assembly command? We never use that. Do you mean
"Create Derived Substitutes" in the "Productivity" of the "Assemble" Ribbon?

Re: A bug in update 3 of Inventor 2019 ?

johnsonshiue — Mon, 18 Mar 2019 23:53:32 GMT

Hi! No, the command is on 3D Model tab in a part. Start a new part -> Derive -> pick the assembly.

Many thanks!

Re: A bug in update 3 of Inventor 2019 ?

Xun.Zhang — Mon, 08 Apr 2019 01:12:42 GMT

Hello @liminma8458,

Johnson is right, this is a behaviour enhancement in 2019.2 with Ticket number INVGEN-4394 internally. It was about to

to solve consistent mass property between source file and Shrinkwrap or Substitute part. In other words, a Shrinkwrap or Substitute part should never use the local geometry to calculate the physical properties. Those should always come from the source assembly.

To your question, please go to Derive workflow as Johnson indicated above.

Hope it helps!

Re: A bug in update 3 of Inventor 2019 ?

liminma8458 — Mon, 08 Apr 2019 21:58:41 GMT

Xun and Johnson, Thank you first. It sounds reasonable for shrinkwrap to have the original assembly physical properties. But after the conversion shrinkwrap becomes a part (a single body without seam and contact surfaces in between) which will be used for further processing, it should also provide some local and true properties for the part itself at least through API. To our application, we need some unique features in shrinkwrap such as " remove hole", "remove pocket", remove chamfer" and so on. So we end up to modify the code to iterate all faces in the shrinkwrap to calculate the full surface of the shrinkwrap part. Should we request that autodesk put back the local surface and mass properties at next release at somewhere? Thanks again.

Re: A bug in update 3 of Inventor 2019 ?

shaoni — Tue, 09 Apr 2019 03:09:13 GMT

Hi Limin,

Could you share more further usages on shrinkwrap part in your work? These can provide insights on whether or not to have an option to always sync physical properties with original assembly.

For the issue you met now, here are two solutions you can try with.

Solution 1:

1. Do Shrinkwrap as usual as you do.

2. New another Part, use Derive to derive your shrinkwrap part in. In this way, you will get local physical properties as you want.

Solution 2:

As you want to use the Simplify options provided in Shrinkwrap. You can try with the simplify features provided in Part, this panel is hidden by default, you need check it on in the show panel list to show it in the 3D Model tab in Ribbon. However, these tools are not as powerful as options in Shrinkwrap. But depends on your models. You can try it out .

1. New a part, use Derive to derive your assembly file in.

2. Show Simplify tools in 3D Model tab. Try with Fill Voids, Remove Details.

Please let us know, Do these 2 solutions help?

Thanks

Nina

Re: A bug in update 3 of Inventor 2019 ?

liminma8458 — Wed, 10 Apr 2019 23:12:48 GMT

Hi, Nina,

Can you give me your email address? We can arrange a remote desktop conversation to show you our application scenario when I come to China for project.

Solution 1 will be practical. For solution 2, when is the simplify features in part mode? I can't find it under 3D Model tab in Ribbon? where is the show panel list? are they from any addin? I am using update 3 of Inventor 2019 pro.

Thanks

Limin

Re: A bug in update 3 of Inventor 2019 ?

shaoni — Thu, 11 Apr 2019 11:26:25 GMT

Hi Limin,

Sounds great, my email is nina.shao@autodesk.com.

To show Simplification panel, you can follow the steps shown in the image below. It was added in Inventor for many years, from Inventor 2013. These tools using different methodology to detect features and remove features, the method in Shrinkwrap is much more powerful. You can try with these tools to see if they work for your models.

Looking forward to meeting you later!

Regards,

Nina