Mirror a view

[johan.degreef]

In Solid Edge I used to copy a view, make it dumb lines and mirror it. is there a workflow in Inventor to copy a view in a drawing and the mirror it without the need of a complete mirrored 3d model?

I need 2 assemblies from this, but 1 mirrored supposed to the other.

[cadman777]

I know of no way to do what you want to do in Inventor. However, you can do it in AutoCAD by saving your Inventor drawing, opening it in AutoCAD, mirroring the desired view, Wblocking it out to disk, and then importing it into an Inventor drawing Sketch. At least that's how I would do it.

[mikejones · Accepted solution]

Possibly depending on the drawing template you use. If you're using the dwg format for drawings rather than idw then there is a workaround that may get what you want.

With the drawing open and saved, under the Drawing Resources folder in the drawing browser you will see the AutoCad Blocks folder.

In that folder, you will find an Autocad block representing each view on your drawing. Insert the blocks that you want mirroring into the drawing; the scale will be full size but you can RMB click the views once placed and go to Edit AutoCad Block and set the scale.

Next, RMB click on the Autocad block view and select Open In AutoCad. You'll get a warning that Inventor needs to close which is fine.

Autocad will open up your drawing where you'll be able to mirror the relevant blocks using standard AutoCAD mirror command. Don't explode the blocks though, that is important! 

Save the file and close Autocad.

Reopen the drawing in Inventor and you have your mirrored views.

The great thing with this though, as long as you didn't explode the block in AutoCad when you mirrored it, is the block views are still associative to the parent so will update with the parent Inventor view

Hope that helps

Mike

[CGBenner]

@mikejones 

Great and well detailed tip, Mike! 

[mikejones]

Thanks @CGBenner.

I think that trick is little known. And it's way neater than the dumb view in SolidEdge.

Mike

[cadman777]

I'm curious as to why you prefer Inventor dwg over Inventor idw to make drawings?

This question might could be a whole topic of its own.

[cadman777 · Accepted solution]

Incidentally, a way I've done this in the past, is to Derive the assembly into a part file, then derive that part into another part file, except bring it in as-mirrored. Then just place the view in the drawing.

The problem with this method is you can't use a PartsList w/this view. It will update according to changes made to the parent assembly, but you can't access any of the single parts, for obvious reasons. In that case, I just manually double the quantity of parts shown in the 'other hand' PartsList. It's not a big deal, since it seldom occurs.

[mikejones]

Mainly because I can send an inventor dwg drawing out to a customer who only has autocad to view in.  Its also possible to pass an already started inventor dwg drawing on to a draughtsman using automatic to finish off whilst maintaining associative.

[cadman777]

Makes sense. It always amazes me that most of the fabricators and customers use "AutoCAD" for information exchange. To me, they're living in the dark ages!

[johan.degreef]

In the end I created a dummy part, and derived it from the original assembly. On derive, I can choose to mirror it pon any axis.

I insert the dummy part in an extra view in my drawing, and it gets updated, every time my original updates as long as I don't break the link of the derived part.

It think most simple way to do this, but thank you for all suggestions.

[jwinkel2396N]

Great tip Mike! I was just able to replicate this. However, I'm having issues with dimensioning. Dimensions are not correct if the block is not full scale, and dimensions are sick as soon as I create them. Have you encountered these issues, and have you been able to overcome them?

[mikejones]

Hi.

I've only ever used this trick to create a mirror of an isometric view without applying any dimensions but I've just tried the process on an ortho view and have the same broken dimensions that you're seeing. Unfortunately, I don't have a work around to that apart from deriving the part and mirroring it as others have suggested.

Mike