Mirrored Part: Doesn't have any parameters and rules

[Anonymous]

Dear colleagues!

I faced a problem when tried to "Mirror" my iLogic parts/assemblies

So, if I have rules and parameters in original elements, I don't have them on the "mirrored" parts!

I have, let's say, solution for this problem (Just do circular pattern) - but this is not correct solution

There are two screenshots: 1 - Original part, 2 - Mirrored part

Waiting for your comments!

[Anonymous]

We ran into the same issue at our office, came up with a workaround.

Start a new part with the template with all of your i-logic and parameters. Use the "derive" function, clicked on the mirror about selected plane feature to create a mirrored part of your original.

You can bring parameters from your original part but not sure about the i-logic though it will be in your template.

[salariua]

Mirror does just that "derives the original with mirror option" so you can open each mirrored part and then use "Edit Derived Part" option on the right click menu.

That will allow you to bring over any other info you need.

[Anonymous]

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@salariua wrote:

Mirror does just that "derives the original with mirror option" so you can open each mirrored part and then use "Edit Derived Part" option on the right click menu.

That will allow you to bring over any other info you need.

---

We use it a lot for sheet metal parts and the I-Logic we use for sheet metal parts does not transfer just using the mirror command.

So we use the template and derive.

Standard mirror command it seems does not give the OP the model he is looking for.

[johnsonshiue]

Hi Artem,

Indeed, the Mirror Component command focuses on geometric replication. It uses Derive command to create the mirrored side. The parameters and rules are still in the source part. Essentially, the source part will always drive the mirrored part.

For the mirror workflow you are looking for, you may consider using Mirror command within the part. Open the part and save it as a different part. Next, use Mirror command -> Solid Mirror -> select the mirror plane -> check Remove Original -> Ok. Now you will get the mirror side of the body. The nice thing about this workflow is that you still have the feature tree, though on the source side. The rule should still run. Would it work for you?

Many thanks!

[salariua]

If you do decide to mirror in the part keep in mind that you will need to modify both parts.

Don't expect the mirror part to update with you original model.

[Anonymous]

Hi, johnsonshiue

!

Thank for your reply!

I didn't understand all the actions to create a mirrored part that I'm looking for

I still don't have solution. It's my own fault, that I don't understand

Could you, please, try to explain a little bt easy for me?

[Anonymous]

Hi, salariua!

Thanks for your reply!

I really tried to do what you said, but I don't have the same rows in the menu after mirror ("part priority")

And I can't find "edit derived part" and so on

May be I have different Inventor version?

Inventor 2017 Professional

Build 256, Release 2017.4

[adam]

I know this in an old post but...

If you have already created a mirrored part and need to bring in the original parts parameters: Open your mirrored part, then right click on the .ipt in the model tree, select "Edit Derived Part" it will open up the Derived Part menu.  Click on the circle icon next to parameters to toggle them on or off.

[Xun.Zhang]

If so, please do not leverage derive workflow. Copy the original part and paste, rename it, open this part again, make a new mirror feature for all features or for solids, then, all parameter and iLogic rule are perserved.

Hope it helps!

[johnsonshiue]

Hi Adam,

To elaborate Xun's suggestion, you want to save as or save copy as the original part. Then create a Mirror Body feature (Mirror -> Body selection -> check "Remove original"). Then you will have a new part with a mirrored body and all features, parameters, and iLogic rules preserved.

Many thanks!

[Manuelcamposcosta]

I might have found a bug when you mirror parts within an assembly if it's a sheet metal one the template of the new mirrored file will not be exactly like the standard.ipt altough for a normal part it keeps all the information the standard.ipt had before.

For example create a plane in your standard.ipt if you mirror a normal part, the new part will have the same plane, but if the mirrored part was a sheet metal it will not create the plane, I think there is some sort of a bug with the template that is being used when we mirror sheet metal parts.

[JDMather]

@Manuelcamposcosta 

This is not the same issue.

It would probably be best if you -

1. Start a new discussion thread

2. Include example files illustrating the behavior.

[johnsonshiue]

Hi Manuel,

It does not sound right to me. As JD mentioned, it could be a different issue than this original thread. If possible, please share an example that exhibits the behavior.

Many thanks!

[Manuelcamposcosta]

I'm focusing in the title "Mirrored Part: Doesn't have any parameters and rules" it's exactly like the title says.

I think it's easier if you try by yourself, because if I send the files you will not understand.

1. Create a template with some sort of an ilogic, some user parameters and create for example a plane in with;
2. Create a sheet metal part and be sure you used the template created before;
3. Create the mirror part but don't use derive command or mirror it with the mirror function of part menu, instead place that part in an assembly then mirror the part using a plane;
4. Notice that the new part doesn't have the ilogic, the plane and the parameters;
5. Repeat 2 and 3 but now for a normal part;
6. Notice that the new part does have the ilogic, the parameters and the plane.

Anyway attached is a template, a normal part, a sheet metal part and their mirrored versions, all created with the same template, but you could try from the start by yourself.

[johnsonshiue]

Hi Manuel,

Yes, I get it. This is about the ability to create fully functional mirrored design. Driven or not driven by the other side should be optional.

Indeed, the current Inventor Mirror Component is geared toward to fully-driven by one side. The workflow to create independent or partially independent mirrored component has to be done manually (use Mirror Body -> Remove original; constrain the components accordingly). It can be further automated, since it can already be done manually.

Many thanks!

[Manuelcamposcosta]

What you are saying is right, but that's not what I'm talking about.

I talking the differences when you use this command for normal parts and for sheet metal parts, in sheet metal parts the template is wrong.

[johnsonshiue]

Hi Manuel,

I see. This particular request is known indeed. However, it is not as straight forward as it sound. The problem is that though the Make Component/Derive command is the same for a regular part and a sheet metal part, there is indeed difference in the actual internal process. The current behavior prevents a mirrored sheet metal part from becoming corrupted. I vague remember discussing it with the project team but there was no straight forward solution unfortunately.

Many thanks!

[Manuelcamposcosta]

Hi,

Ok so it's not a problem with my template, currently it's a limitation, right?

[johnsonshiue]

Hi Manuel,

Indeed, it has nothing to do with your template. It is not your fault. It is the way the Make Components dialog is structured making the workflow a bit less intuitive.

Many thanks!