Disappearing Dimension on .idw

[chrisw01a]

Ok, here is a new one with Inventor 2018.

When adding a dimension to a drawing view, sometimes I need to turn on hidden lines to get the correct dimension.

Afterwords, I will go back and turn off hidden lines because it is not necessary and it clutters up the view.

Before, the dimension would be fine.  Now it disappears after I change the view back.

I am really hoping there is a setting for this somewhere.  Can anyone help with this?

Thank you all so much for your help lately...

Chris

[JDMather]

Rather than dimension to hidden lines (and in this case "missing" hidden lines) - I would do a Break Out Section of that feature.

[chrisw01a]

That would work I suppose.  

I didn't know if this was done by design or what since it has been the same since we started using inventor 15 years ago.

Thanks for the idea.

Chris

[Mark.Lancaster]

@chrisw01a

One thing to test..  In your drawing, go to Tools/Document settings and enable preserve orphan annotations.  If that leaves your dimensions that's an indicated you are creating an orphan annotation by changing the layers.

[chrisw01a]

I tried this and still the dimension disappears.

Thanks

[johnsonshiue]

Hi Chris,

I believe the behavior was changed as part of defect fixing. Some users complain that dimensions to hidden line edges should be hidden when the hidden lines are not displayed. Now, when the hidden lines are removed, the associative dimensions will be hidden. When hidden lines are calculated, the dimensions will be back.

Many thanks!

[SBix26]

I sure wish that had been made an optional "feature"!  I rarely use it, but dimensioning to hidden lines is a very quick and efficient way to get a dimension where otherwise it may require a sketch.  This most often applies in isometric views.  So this user is now complaining that I don't want my dimensions to automatically disappear when I hide the line they're dimensioned to.

I'm very disappointed to know that I now have no recourse in those situations but to create a view sketch.

Now what happens in the case of a view sketch where a sketch element is used for a dimension, and then the element is changed to Sketch Only?  Does the dimension become invisible in that case, too?

When was this change made?

Sam B

Inventor Professional 2017.4
Vault Workgroup 2017.0.3
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

[chrisw01a]

Very well said and exactly why I created this post.  I use this same workflow almost daily for quick proposal drawings.

I hope something can be done about this.

chris

[Anonymous]

---

@johnsonshiue wrote:

Hi Chris,

I believe the behavior was changed as part of defect fixing. Some users complain that dimensions to hidden line edges should be hidden when the hidden lines are not displayed. Now, when the hidden lines are removed, the associative dimensions will be hidden. When hidden lines are calculated, the dimensions will be back.

Many thanks!

---

For every person who complains about a feature's behavior, there are ten who will be disappointed when you "fix" it. 🙂  I do sympathize.

[chrisw01a]

Do you know if there is a registry edit for this?

[johnsonshiue]

Hi Guys,

Indeed, like I indicated earlier, it was indeed fixing a legacy defect about hole table. When a hole table (or dimension) was associative to hidden line geometry, it remained visible after the the hidden lines are removed. We had received complaints about the behavior and we made the change in 2018. It would have been better if there is a switch to control the behavior (default to current behavior). I will work with project team and see what can be done. But, unfortunately there is no way to control the behavior. Any dimension or annotation associative with hidden line geometry will be hidden when hidden lines are removed.

Many thanks!

[SBix26]

What about Sketch-only geometry?  That is, sketch geometry placed purely for dimensioning, then changed to Sketch-only so it's not visible?

I don't have 2018 operational yet, so I can't check it for myself.

Sam B

Inventor Professional 2017.4
Vault Workgroup 2017.0.3
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

[andrew_faix]

Hi everyone,

Long before I started at Autodesk, I was a mechanical draftsman (sorry....draughtsman).  I've been pretty well schooled that dimensioning to a hidden line at all (regardless of it's visibility state) is an absolute rule violation.  Until I read this discussion thread, I would have thought that was a fairly hard and fast rule regardless of standard / geo / industry.

OP wrote:

"...sometimes I need to turn on hidden lines to get the correct dimension"

That's the kind of statement that would have made my CAD manager cringe.  This seems like a very error-prone practice.  Moreover, we've worked pretty hard to implement tools to address this need without having to rely on, what would be generally regarded, as bad drafting practices.  Specifically: you can obtain the "correct" dimension with a section or break-out view (in the screen-capture provided, a break-out view seems best).

Later in the thread:

"...dimensioning to hidden lines is a very quick and efficient way to get a dimension where otherwise it may require a sketch."

Again - no sketch required here.  There's a specific tool to solve this problem (either in ortho or isometric views): break out view (ok - well...sketch is needed to define the break-out region).

Isn't making use of break-out or section view a more standard and less error-prone solution to this problem than dimensioning to hidden lines?

Thanks,

-Andrew

[chrisw01a]

Thank you for the information.

[chrisw01a]

Andrew,

I understand what you are saying however when all we require is a quick reference dimension (nothing critical) it works out very well.

This was generally done on "proposal" drawings for customers where general overall dimensions were given simply to illustrate the intended size of the product.

If I were detailing out a drawing for fabrication, that would be a different story.

Nevertheless, I'm sure we will adapt and move on.

Thanks for your input.

Chris

[SBix26]

Here's an example of a situation where I dimensioned to a hidden line.  This is an aluminum T-slot extrusion frame.  The left end of the 25.75 dimension is made to a hidden line, without the mess and additional fuss of a breakout view.  I don't think there's any ambiguity in this dimension (at least the vendor I sent it to for a quote didn't seem to think so), and this is an example of the fairly rare situation in which this is by far the most efficient and clearest method to dimension something.

In general, I agree that dimensions should not be to hidden lines, even when they're visible in the drawing; but sometimes this technique is the simplest way to produce a proper drawing.

Sam B

Inventor Professional 2017.4
Vault Workgroup 2017.0.3
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

[chrisw01a]

Well stated.  Thank you.

Chris

[andrew_faix]

Thanks for the additional information everyone.  The "best practice" discussion is academic.  What this may come down to is an over-zealous solution to what was specifically a problem w/ Hole Tables (as Johnson alluded).  We're continuing to look into this matter.

[chrisw01a]

Thank you.  If you find a way to change it back let us know.  Lol.

Chris

[Andrzej.J]

Hi Johnson,

I have just read what you write below, and .... I think you must be joking 🙂

And which is true:

1. Status:This incident is being investigated for a possible cause and resolution.
   Additional Information:Article #000122586
   Defect Tracking System: FTS
   Incident id:182437
   at
   https://knowledge.autodesk.com/support/inventor-products/troubleshooting/caas/sfdcarticles/sfdcartic...
   
   OR
   
   
2. Your curious explanation below?

I am writing a yearly book for engineers about Inventor 2018 and trying to annotate typical mechanical drawing. And the conclusion is "I cannot do it in Inventor 2018".

Please watch the MP4 enclosed

I hope the #1 is true and the proper-previous solution will be back soon.

Regards,
Andrzej

Andrzej Jaskulski | mobile: +48 602 65 39 98
andjask@evbox.pl | andjas@uwm.edu.pl | http://www.uwm.edu.pl/acs | http://cadaj.blogspot.com | http://www.youtube.com/user/andjask