Inventor 2013 Sheet metal flat on Mirrored part issue

[Retrodenizen]

Hello,

I have been looking through the forums for an answer to an issue I'm having, but I cannot seem to find one that seems to want to work for me.

My problem is such.  I have a sheet metal IPT that I saved, then did a saveas and saved as a different file name.  I then took the part in the new IPT and did a mirror on the part.  I chose the second "Mirror a Solid" option in the mirror dialog box, and clicked "Remove Original".  Now that I'm at this part, when I try to make a flat patten of the new mirrored part, all I get are the bend and center lines of the part, not the internal and external lines that I can export for use in water/laser cutting.

I was wondering if I was doing something wrong in order to make this work.  In looking through the forums I have seen people say not to use the mirror command in an assembly and create a derived part because that has issues, but I did this in an IPT, not an IAM.  I have also read to make sure that the Sheet Metal Defaults are set the same, but I believe that they are talking about the derived part from an IAM drawing.  All the same, I have checked my Sheet Metal Defaults and they are all the same, and in fact I tried updating them to see if it would still change the part, and it did.  I was able to make my part other thicknesses and it updates the part as per the norm.

I am using Inventor 2013 Professional, if it matters at all.  I have attached the file in question.  I have also attached a couple of picture files showing the part folded and how it looks to me when I go to the flat pattern.  If anyone could point me in the correct direction to go to look for answers, or has answers and are able to help me, please let me know.

Thank you.

[blair · Accepted solution]

Delete the Mirror in your RH part, add the two features again. Save and close your RH Part. Start a new Sheet-Metal part. Don't create any sketch, select the 3D Model tab and select the Derive icon. Then select the RH part in the select dialogue box, make sure you have the "Mirror" selected. This will now create your LH part. All you will need to do is make sure that the Sheet-Metal Set-Up is set to the correct material and thickness. You should now be able to create your flat pattern.

You LH part is now linked to your RH part, any edits done on the RH part will show up on the LH part. If you don't wish for the LH part to be linked, RMB on the feature in the browser and select the suppress or break link.

[jingyi.liu · Accepted solution]

Hi

I checked your model, the root to cause flat failure were face2/face3 when you tried to change the gap of the corner.

Indeed, you can expand Feature Flange4, and edit the node of Corner 4, change the gap setting by inputting the size of gap. see below image.

Then you can flat the mirrored part.

[jingyi.liu]

Hi Matt

Here is the part for your reference.