Selecting a specific end point at line intersection while dimensioning

[petr_vonasek]

I have a simple view with some dimensions. After I change model parameters the view reflects the change and the dimensions (mostly angular) are often detached (are sick = purple). I can of'course reattach them manually but it is frustrating because the model and drawing are the "base source" and I often copy them to many ongoing orders and modify them. Normally I create angular dimensions by selecting 2 lines.

Initial view (dimensions are OK):

After model change (dimensions are detached):

What can help:

For linear dimensions it is better to select the line itself than its end points.

For angular dimensions the only method I discovered is switching off the visibility of 2 short angled lines and create the angular dimensions by selection of the 3 marked end points. Afterwards I have to switch on the visibility of 2 short angled lines again. It consumes lot of time repeatedly.

The cause is:

During dimensioning when I want to select end point at intersection of 2 or more lines, now there is no possibility to decide (select) end point of what line the dimension shall use and Inventor selects the line (and its end point) randomly.

Suggestion:

When I hover the cursor above the marked point while dimensioning, I would like to have a chance to decide end point of what line (either 1 or 2) the dimension shall use. Because some of the lines are more stable than others depending on model feature history.

The line selection might be provided via RMB menu when the cursor is (while dimensioning) above the marked intersection point.

[jhackney1972]

I cannot reproduce your situation where the sick dimensions are created.  I placed the dimensions using the selection of lines which automatically finds the endpoints due to my snap settings.  Take a look at my screencast and see if I am missing something.

If you want to peruse this idea, a better place for your post is the Inventor Idea Station.

[rhasell]

Hi

I know what you mean, but it is hard to reproduce.

I get it a lot, the angular dimensions have to be deleted and re-done, also any orphaned hole notes have to be deleted and re-done.

I have been thinking about this, maybe you could try "Retrieved dimensions" so the model is now driving them, instead of the drawing?

The other option is also "Retrieved dimensions" from the Sketch you made in the drawing view? As long as the sketch is stable, the dimensions should theoretically follow.

In my environment, I don't do this enough to warrant a work-around, its just an irritation, so I live with it, if this happened every time, I would find a work-around, as in your case.

[jhackney1972 · Accepted solution]

I tried the same test using, as you suggested, retrieve model dimensions and I still cannot replicate your issue.  I guess I will just be thankful and hope that you can come up with a "usable" solution.

[jan.vonasek]

The issue happen because side lines are replaced by another side lines due to different model operation. So side line are not stable. Only way to do stable dimension is to use top and down lines or theirs end points.

Solution seems to be ability to select which line will be used as source for selected point.

[petr_vonasek · Accepted solution]

One important information:
I used skeletal modeling (skeleton + multibody part + create components  ). This "hoop" has 2 angled edges created by Split tool with work plane. Bent part has sometimes open angle, sometimes close angle. Also the angle of the work plane is often different = different angle in side view.

In this case Inventor recreates the short angled edges after each model change and therefore the dimensions detach from the geometry.

In this case only the long horizontal lines are stable enough to prevent detaching the dimensions. But there is no option to select just their end points while dimensioning.