Inventor 2019.X flat pattern view in idw does not match model

[cadadmin]

Hello,

 Attached is another example we have where flange bends/notes are lost in Inventor 2019.X. In the Over Shelf Mid RT 2 Piece Kncl Jnt _dd00092.idw, look at the flat pattern on the right hand side, note the absence of bend lines and or geometry, the dimensions to the bend lines are not flagged as dangling(pink). If we open up the Over Shelf Mid RT 2 Piece Kncl Jnt _dd00092.ipt there are no indicators that the flat pattern has issues nor the folded model. We caught this because our custom VBA that computers entities on the flat pattern to automate some processes threw errors (OUT OF BOUNDS).

 I deleted the flat pattern and recreated it in Over Shelf Mid RT 2 Piece Kncl Jnt _dd00092_2.ipt and the corresponding .idw. As you can see it now creates the flat pattern view in the drawing correctly. Just placing a new flat pattern yielded the same result, so deleting the flat pattern and recreating it is a requirement. While the files state they have been created in Inventor 2016, I know that the person who originally created it has not worked for us in some time. If I had to guess, I would say this file was most likely created in Inventor 2014 or prior. One of the things I have not seen is notices to delete the 2011 (I believe that was the year) flat pattern on legacy parts.

I will add there is/are some oddities with the files, there is only a “Master” view, and some of the views were not set to associative. So while I feel like this is an Inventor issue, there was some obvious “poor drafting practices” involved. For illustrative purposes I did not dimension everything and some details have been removed. I believe at this time I am leaning to changes in the sheet metal portion of inventor as well as potential translation issues when opening legacy parts. I would appreciate any input provided.

Regards,
Tom

[johnsonshiue · Accepted solution]

Hi Tom,

This is indeed a bug. We had attempted to fix it on 2019.4 but the fix introduced more issues. So, it was backed out. There is something unique about the affected sheet metal part. Some bends were created in the old algorithm which might be problematic.

For this particular case, there is a quick workaround. Open the part and go to Manage -> Rebuild All. And, edit Flange3 and then uncheck "Old Method" at the bottom -> Ok. You will see the part is unchanged but the bend lines will appear in the drawing.

Could you try it on your machine and see if it works?

Many thanks!

[cadadmin]

Johnson,

 Thank you, that did work with this sample. We have many legacy parts as well as new parts that use the "old method" so we look forward to a fix. Thank you! As we are constantly reviewing our drafting methods, at this time should we look at discontinuing usage of the "Old method"? 

Regards,

Tom

[johnsonshiue · Accepted solution]

Hi! Except on the old files, for any forward created part, I would avoid using Old Method. That option was there to help older feature version to migrate to newer version. It is better to use the new methods without checking the box.

Many thanks!