Inventor assembly mirror

[psw1125]

Hello?
My name is SW Park.
I have a question about the Inventor assembly.
I currently have an assembly with about 1000 parts.
I want to mirror this assembly as a whole to create one new assembly.
Can you tell me how to do this?

[SharkDesign]

Several ways to do this depending on what you want. 

If you literally want all the files mirrored, use mirror from the pattern tab.

You can also select files you don't want mirroring in here.

You get the option of putting those files into the current assembly or into a new one. 

They will update when the original part updates. 

If it's just for a reference file, you can use derive and it will make mirrored dumb block versions of your files. These will always update when geometry changes. 

[psw1125]

thank you for the reply. Mr. jameswillo

Is there a way to avoid adding _MIR to the end of the part name after the assembly is mirrored?

If I clear the _MIR from the options, I get an error saying it's the same name.
And I want the drawing to be automatically updated to fit the symmetrical part, is there a way?

[SharkDesign]

Yes, in the mirror dialogue wizard, it shows you what it's going to call the new files. 

You can change the suffix at the bottom to whatever you want or turn it off and manually edit the names. 

You can't have the same names because Windows won't let you have two files in the same place with the same name. 

(Unless you change it in the wizard to have a different location. But why would you want the same name?)

It won't copy your drawings for you. You can try doing a save as on the drawings and 'replace model reference' but I don't think you'll have any luck with that. 

The only way I've seen it done with the drawings, is to manually go into every part and do a mirror operation of the full solid. You still lose a lot of references in the drawing, but you can reattach the dimensions. 

[psw1125]

Thanks for your reply. I have an additional question for you.
After mirroring, the mirrored part is connected to the original, is there any way to break it? I would like to have a model tree like the original (eg extrude, revolve, hole, etc).
After mirroring the assembly to get the part, is there a way to check if the part after mirroring is the same as the part before mirroring?

(In the case of a symmetrical shape, I know that when a part is symmetrical, it becomes a part of the same shape.)

[SharkDesign]

You cannot do it to show the model tree. You would have to open every part separately and perform the mirror at part level. 

You can break it, but I recommend suppress in case you want to refresh it from the original. 

Open the mirrored part on it's own, right click in the browser and choose 'suppress link.'

'Break link' cannot be undone, but suppress can be turned off. 

You can use direct edit on a mirrored part to edit it, but not have access to the sketches and features like you are asking. 

[johnsonshiue]

Hi! I believe you would like to have a brand new set to components on the mirrored side, right? There isn't an one-click button to do that. You will need to do it on an individual part basis. First, you will need to make a copy of the the entire assembly using iLogic Design Copy (Design Assistant or Vault Copy Design).

Second, open each part and create a Mirror feature -> Body -> Remove original. In this way, the part body will be mirrored to the other side, which all the features and parameters remain there.

Lastly, fix the assembly constraints accordingly.

Many thanks!