topic Re: Problem with the mirror feature to maintain the positions of the original component in Inventor Forum

Problem with the mirror feature to maintain the positions of the original component

apoiotecnico7Q2PQV — Fri, 09 May 2025 17:47:12 GMT

I have a question about the mirror feature in Inventor. Every time I make positioning changes to the original part that has been mirrored, the other part doesn't follow the changes. How can I solve this problem without having to reposition the mirrored part again? The purpose of the mirror feature is to generate another part inside the assembly that continues to have the same relationships of the original part selected in the feature. That's why I kept the + symbol in the command setup.

Re: Problem with the mirror feature to maintain the positions of the original component

CCarreiras — Fri, 09 May 2025 18:09:08 GMT

Boas,

1)If you are using Inventor 2026, it will work like you expect. If you change the source position, the mirrored part will follow that change as a mirror. (It's a new update for the Mirror tool).
2)If you are using Inventor 2025 or below, the mirror will place the mirrored part well placed the first time, but the mirrored part will be locked in position (grounded).
If you intent to change the source part position and expect the mirrored part follow that change, you will have to unground the part and add additional constrains.
Tip: in that cases, i used to apply symmetric constraints between the source part geometry, the mirrored part equivalent geometry, and the mirror plane.

Re: Problem with the mirror feature to maintain the positions of the original component

apoiotecnico7Q2PQV — Fri, 09 May 2025 18:47:40 GMT

Thank you for your reply! However, I currently have the 2026 version and the mirrored part still doesn't go with the original one. Would you recommend doing the same as your answer for the 2025 version? If so, what's the difference between that and making a copy of the part, and positioning it again?

Re: Problem with the mirror feature to maintain the positions of the original component

kacper.suchomski — Fri, 09 May 2025 19:35:43 GMT

In the Mirrors dialog box, you must make the appropriate settings to preserve associativity.

Since you did not share the files, we do not know what you did or did not do.

Re: Problem with the mirror feature to maintain the positions of the original component

johnsonshiue — Fri, 09 May 2025 21:22:37 GMT

Hi Carlos and Kacper are right. Mirror Components should just work in 2026. Please share an example that illustrates the behavior here. I would like to understand it better.

Many thanks!

Re: Problem with the mirror feature to maintain the positions of the original component

CCarreiras — Mon, 12 May 2025 09:19:38 GMT

Hi!

It should work in 2026 version.

Is this it, what you are trying to achieve?

(view in My Videos)

Re: Problem with the mirror feature to maintain the positions of the original component

CCarreiras — Mon, 12 May 2025 09:58:22 GMT

@apoiotecnico7Q2PQV wrote:

what's the difference between that and making a copy of the part, and positioning it again?

A) Copying a part will give you two options:

1) Create a new part which is equal to the source, but is a new file(blue)

2) Repeat the same file in the assembly, the same as place the same part again manually (reuse option - Yellow)

,,,and you can place both cases anywhere in the 3D space then you must apply constraints.

B) Mirroring a part will give you two options:

1- Create a new part, which is a source mirrored part (green)***

2) reuse the source to create a repetition (Yellow)

...and for both cases, the new or repeated parts will be automatically positioned regarding the mirror plane.

(view in My Videos)

*** some parts, when mirrored, need to be a new part, cannot be reused. The Mirror tool will do that for you, create a new part which is a mirrored source geometry.

Here's an example where you need to mirror the part itself (green - create a new part which is the source copy, but mirrored) along the mirrored positioning.

(view in My Videos)

Tip: consider to have some Inventor training.