topic Re: Serious drawing dimension issue when starting from non-ortho view in Inventor Forum

Serious drawing dimension issue when starting from non-ortho view

-niels- — Mon, 28 Jun 2021 14:21:03 GMT

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.

Re: Serious drawing dimension issue when starting from non-ortho view

bradeneuropeArthur — Mon, 28 Jun 2021 14:33:55 GMT

Are you using this setting?

Re: Serious drawing dimension issue when starting from non-ortho view

-niels- — Mon, 28 Jun 2021 14:46:48 GMT

@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?

Re: Serious drawing dimension issue when starting from non-ortho view

bradeneuropeArthur — Mon, 28 Jun 2021 14:57:36 GMT

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!

Re: Serious drawing dimension issue when starting from non-ortho view

SBix26 — Mon, 28 Jun 2021 15:08:14 GMT

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

Re: Serious drawing dimension issue when starting from non-ortho view

johnsonshiue — Mon, 28 Jun 2021 18:51:39 GMT

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!

Re: Serious drawing dimension issue when starting from non-ortho view

bradeneuropeArthur — Mon, 28 Jun 2021 19:16:04 GMT

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

Re: Serious drawing dimension issue when starting from non-ortho view

-niels- — Tue, 29 Jun 2021 06:13:29 GMT

@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!

Re: Serious drawing dimension issue when starting from non-ortho view

SBix26 — Tue, 29 Jun 2021 17:04:11 GMT

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

Re: Serious drawing dimension issue when starting from non-ortho view

alysia.devries — Wed, 16 Mar 2022 04:13:55 GMT

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!!

Re: Serious drawing dimension issue when starting from non-ortho view

-niels- — Wed, 16 Mar 2022 07:15:40 GMT

@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.