If feature is dimensioned I cannot use the trim tool

[mcarroll6VECD]

I am creating a new standard part.  It's a rectangle that I need to detail out some notches.  However, when I start to create the notches I get the following error.  I am coming to inventor by way of Solidworks, then fusion 360. 

This is the error message:

"The curve being extended, trimmed or split has a dimension. Remove the dimension to perform the operation."

How to replicate.

1. Draw rectangle

2. Dimension.

3. Draw inner rectangle to trim out a notch

4. Press "X" to trim

5. Using the mouse to trim lines as illustrated by the pink box in the attached illustration. 

[JDMather]

When you Trim, if you click on the line (rather than hold and swipe) it should trim the line.  

Then Delete the shorter line.  (You will have to add a coincident constraint, same as in SolidWorks.)

But if you are using Inventor 2020 or later (or using SolidWorks) in general you can select the desired profiles (Contour Select) when creating feature without trimming anything.

[johnsonshiue · Accepted solution]

Hi! It seems like a change in behavior recently. In the past, when you trim off the line, the associated dimension will be deleted automatically. This behavior was nice if you don't care about the dimension. However, it can be problematic if the dimension is being reference elsewhere. I suspect an additional check was added to prevent the dimension from being deleted. If you want to trim the segment, you need to manually delete the dimension. Then trim it.

I will check with the project team to confirm the behavior.

Many thanks!

[Xun.Zhang]

Hello @mcarroll6VECD ,

In the step 3, try to draw two perpendicular lines rather than a rectangle, it will work.

Hope it helps!

[mcarroll6VECD]

Johnson, you said:

"If you want to trim the segment, you need to manually delete the dimension. Then trim it."

that is what I am finding is working.  I seemed to get into a good rhythm in setting and deleting dimensions and then deleting and trimming. 

Thanks.

[mcarroll6VECD]

Xun,

Yes, I agree that this would work, but I also needed to have three sides to form a groove as illustrated in my pics. 

The square allowed me to just delete one segment. 

My process that worked:

1. Dimensions the length

2. Then Delete the length dimension

3. Open the squares up

4. Re-add the dimension

This worked

[jeffg28CLY]

@johnsonshiueDid you find out anything from the project team on this? Is it a setting that can be changed, or is it the way things will be going forward?

I'm on 2021.2 and running into this. I'm coming from Creo, and that didn't care if a sketch entity was dimensioned or not, trim got rid of the thing and its dimensions.

If it's not a setting, is there another option? Maybe something like Shift+Trim to forcibly trim a dimensioned line?

[SBix26]

Another way to preserve the dimension is to change the existing line to Construction, then add the notch geometry.  It will require more lines to connect the notch, but at least the dimension is preserved.  Also, as @Xun.Zhang  wrote, don't use rectangles for the notches, but perpendicular lines (click/drag from an existing line to get a perpendicular one).

Or, make sure when dimensioning your rectangle that you select the two adjacent lines, rather than the line by itself.  That dimension would be preserved when trimming.  That is, dimension the length between the two parallel end lines instead of between the two end points of the long line.  Hope that makes sense.

---

Sam B
Inventor Pro 2021.2 | Windows 10 Home 2004
LinkedIn

[johnsonshiue]

Hi! I think I was mistaken. There is no behavioral change. It has been like this. Like Xun explained before, there are ways to avoid it from happening. But, there isn't an option to avoid the behavior unfortunately.

Many thanks!

[controlsgirl]

@SBix26 That tip about the click and drag is AMAZING!!! Is there a good resource for more tips like this?

[controlsgirl]

Grr nevermind. I drew a line. I clicked it and dragged and it just moved it. 😞

[SBix26]

The Line tool has to be active for the click-drag to work.  Sounds as if after you placed the line, the tool got cancelled.

I don't know about a resource for these shortcuts, but click-drag also works to create a tangent line from a curve.

---

Sam B

Inventor Pro 2022.2.2 | Windows 10 Home 21H2

[controlsgirl]

I stayed in the command. It lets me click the endpoints or midpoints and it'll start drawing an arc, which is nifty, but it isn't letting me drag for a parallel line. Could you upload a screencast to show it? (If you don't have Autodesk Screencast I highly recommend it.