Serious drawing dimension issue when starting from non-ortho view

[-niels-]

My colleague mentioned he saw some strange behavior when dimensioning 2D drawings where it seemed he was getting wrong/crooked dimensions on his ortho views.

After looking into it we found the following workflow that causes this issue:

• Have a part with differences in depth and create a new drawing.
• Make sure to start out with an isometric view or custom orientation that is not orthogonal
• Edit the view to make it orthogonal
• Dimension from a line/point to another line/point that has a depth difference.

This should give an isometric dimension in an orthogonal view, which is unexpected and, depending on if it's a small difference, can go unnoticed.

When placing a a view and starting out orthogonal this behavior isn't present.

This is on IV2021.3.1

@johnsonshiue i've attached my testpart, but it's easy enough to recreate with other geometry as well.

Can you confirm this behavior and see if it's present in IV2022 as well?

We would love to see this fixed.

[bradeneuropeArthur · Accepted solution]

Are you using this setting?

[-niels-]

@bradeneuropeArthur Nope, i never checked that menu.

It is set to "True" when starting from the isometric view.

So i guess that changes the problem to: "why doesn't it automatically change to projected when using an ortho view?"

There is no clear indication that this happens and, once you've place dimensions, changing this setting doesn't adjust existing ones.

Thanks for at least making me aware of this setting and its effects! 😎

Judging by my colleagues workflow this won't be easy to keep track of, so i'm wondering how this could be prevented if the behavior cannot be changed...

Any suggestions?

[bradeneuropeArthur]

No this is often random the case!

Manual reset is the only option!

Edit the existing dimensions is needed indeed!

Would be grateful that this was solved with newer releases!

It has been there since I know for a long time!

[SBix26]

It's easy to follow the logic that makes Projected the default for ortho views and True the default for non-ortho views.  And I can see why the Projected/True attribute is per dimension-- it's possible to imagine a scenario when you might want both in the same view (though extremely rare). 

But something needs to be revised so that these kinds of problems don't happen, or are easily noticed.  If nothing else, simply a notification to pop up and be acknowledged whenever transitioning a view from ortho to non- or vice versa.  Better yet a notification, if there are existing dimensions, plus changing the default setting for that view.

All the more complex if the part is not oriented to the orthogonal planes in its part file to begin with!

Perhaps you could formulate a proposal and put it in the Inventor Ideas forum?

---

Sam B
Inventor Pro 2022.0.1 | Windows 10 Home 20H2
LinkedIn

[johnsonshiue]

Hi Niels,

Arthur and Sam are right. This is the standard behavior when the view is not based on orthogonal directions. This is because the dimensions can depend on the view direction. By default, it sets the dimension type to True instead of Projected.

Many thanks!

[bradeneuropeArthur]

You can run this on save:

Dim d As DrawingDocument = ThisDoc.Document
Dim s As Sheet = d.ActiveSheet
Dim dv As DrawingView 

For Each dv In s.DrawingViews
	If dv.GeneralDimensionType = GeneralDimensionTypeEnum.kTrueGeneralDimension'.kProjectedGeneralDimension
		
		dv.Label.FormattedText = dv.Label.FormattedText & " TRUE PROJ"
		dv.ShowLabel= True
	End If
	
	Next

or this:

Dim d As DrawingDocument = ThisDoc.Document
Dim s As Sheet = d.ActiveSheet
Dim dv As DrawingView 

For Each dv In s.DrawingViews
	If dv.GeneralDimensionType = GeneralDimensionTypeEnum.kTrueGeneralDimension'.kProjectedGeneralDimension
		
		dv.GeneralDimensionType = GeneralDimensionTypeEnum.kProjectedGeneralDimension
	End If
	
	Next

[-niels- · Accepted solution]

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@SBix26 wrote:

Perhaps you could formulate a proposal and put it in the Inventor Ideas forum?

---

I've posted an idea, feel free to add more suggestions to mitigate the issue:

https://forums.autodesk.com/t5/inventor-ideas/idb-p/v1232/tab/most-recent

And add a vote ofcourse.  😉

Thanks for all the input people!

[SBix26]

Here's the link directly to @-niels- 's idea: Indicate if a drawing view is set to "true" or "projected" dimensions. - Autodesk Community

---

Sam B
Inventor Pro 2022.0.1 | Windows 10 Home 20H2
LinkedIn

[alysia.devries]

Since you all seem to be aware of my problem, I thought I’d post here first. I’m trying to dimension a diagonal line in a non-orthogonal view.  If I use one of their ISO views, it actually tells me I can’t dimension it! But if I use the Home or a personalized view that is non-orthogonal, it lets me but the dimensions are not correct.  I’ve read about this “General Dimension Type” selection but it is nowhere to be found when I right click.  Can anyone shed some light on what I’m seeing?  I am using the latest version of the Free For Personal Use software.  Thanks!!

[-niels-]

@alysia.devries Your screenshot looks like Fusion 360, if it is then you should post your question over on the Fusion forum: https://forums.autodesk.com/t5/fusion-360/ct-p/1234

I expect the behavior in Fusion is different from Inventor and any related settings are named differently or in a different location, if available at all.