How to trim both sides

[pawelzdon]

How can I trim a straight element (IPE 100) on both sides when it is bounded by the same curved element (U 100)? The Trim/Extend command only works on one side of the straight element, and repeating Trim/Extend command does not work for the other side.

[kacper.suchomski]

Hi

You can do it this way:

[pawelzdon]

This method returns an incorrect length.

[CCarreiras]

Hi!

It should work:

What version are you using?
Have you all the updates installed?

(I used Inv 2025.3)

[pawelzdon]

I’m using Inventor Professional 2025.2.1. I don't see the 2025.3 version available.
I’m following the exact same steps, but the Trim command only works on one end of the element.

[SBix26]

I see the same result in 2025.2.1, and also in 2026.0

However, I discovered a workaround: open the curved member and use Thicken to add a surface coincident with the face you wish to trim to.  Then back to the frame and add a new Trim-Extend feature for the untrimmed end using the new surface instead of the original face.

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Sam B

Inventor Pro 2026 | Windows 11 Home 24H2

[pawelzdon]

@johnsonshiue, any idea how to solve this? Maybe this is a defect that needs to be reported?

[johnsonshiue]

Hi! 2025.3 is just released. I vaguely remember there could be fixes addressing the exact issue. Please install 2025.3 and see if it works better.

Many thanks!

[pawelzdon]

I installed the version 2025.3, but the issue still exist.

[johnsonshiue]

Hi! Many thanks for trying in 2025.3! I see the same behavior. I think I know where the problem is. Inventor Frame Gen gets confused when the cutting face go across the same frame member twice. Try this and see if it works better for you. Open the arc piece and create an offset workplane intersecting the arc frame. Use Split command and select the workplane to split the arc frame member faces. After that, the Trim will work on both sides.

Thanks again!