How to separate two mirrors

[Anonymous]

I've been making a part in inventor that worked flawlessly, and I had to make an identical part, but mirrored. I used the mirror tool and I need to make a .idw file of both left and right. My problem is, my part is only made in the left side, and I need to separate it to the right alone. I've tried split, but it doesn't work.

If there is a solution to this, please let me know. Thanks.

[mcgyvr]

Edit the feature.. Mirror the solid instead of the feature with the new solid option so that a new solid is created..

Then use the "Make Part" command (manage tab) to push that part out into its own file..

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2016...

Or delete the mirror..

Place the part into your assembly and then use the mirror command at the assembly level to create the mirrored version..

[NigelHay]

Not sure why the split will not work but you can mirror to create a new solid & delete the original. You can create your 1st part, save a copy as a new part then create the mirror. The attached part is the mirror (as a STEP because my Inv is a later version). The JPEG shows the command.

[Anonymous]

Thanks!

[mcgyvr]

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@Anonymous wrote:
Thanks!

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@Anonymous 

You are welcome..

If any of the replies here have answered your question please click the "accept as solution" button under that reply so this thread will be considered "solved" to finalize it and keep Autodesk from sending you an email asking if your question is solved or Kelly or the other Autodesk members from posting more seeing if you still need help.. Just keeps the forums organized,etc...

[johnsonshiue · Accepted solution]

Hi! There are multiple ways to do this. The ability to split two disjoint lumps into two bodies using one non-intersecting workplane is only available on 2017 or 2018 and later. It is not available on 2016.

Like other experts mentioned, you could edit the Mirror and change it to Mirror Solid -> New Solid. Then the mirrored side will become a separate solid. You can create two design views. One with the left side visible and one with the right side visible. Then document them in the drawing.

Or, you don't even need to create the mirror. You simply create two views in the drawing. One view is based on the front and the other is based on the back. The one from the back may show edges in hidden lines. Window-select the edges -> Annotate -> Layer combobox -> assign them to the default Visible layer.

Many thanks!

[rayessle]

Instead of mirroring the solids/features in the part you can derive the part into a new part with the mirror option. you then get the new part which is linked to the first part. If you have to modify the first part then the second will automatically update (and the 2nd drawing).

Regards

Ray Esslemont

Inventor 2018