Dimensions on IDW do not show the correct values.

[Raider_71]

Hi all,

Please have a look at the drawing file under customer files - 4-12-2007.zip. The dimension values do not show the correct values. I have circled them with red markers.
This is a part with compound angles, so I think the problem is that Inventor is applying Isometric dimensioning like when you dimension a projected isometric view. I have verified this by measuring the distances in the model.
I would like Inventor to give me projected/2D dimensions. This issue has only started happening in version 2008 since Isometric dimensioning was introduced. It has cost us quite a bit of money to date and a workaround or fix would be highly appreciated!

Thanks Pieter

[Anonymous]

With the introduction of isometric dimensioning, they also added a flag
for turning it off. If you RMB on a view, look for the context menu item
"General Dimension Type" submenu and set it to Projected. I believe you will
then need to re-insert the dimensions again. This has been discussed
here before, but I know the search tool does not always turn up the
correct results.

Bob S.

Raider007 wrote:

[Anonymous]

There's also a registry setting you can change so that the default setting
for dimensions is ALWAYS 2D projected rather than True dims:

HKEY_CURRENT_USER\Software\Autodesk\Inventor\RegistryVersion12.0\Applets\DrawingLayout\Preferences\DrawingFormat\2DDimensioningOnAllViews
Change from 0 to 1


"Bob S." wrote in message
news:5791968@discussion.autodesk.com...
With the introduction of isometric dimensioning, they also added a flag
for turning it off. If you RMB on a view, look for the context menu item
"General Dimension Type" submenu and set it to Projected. I believe you will
then need to re-insert the dimensions again. This has been discussed
here before, but I know the search tool does not always turn up the
correct results.

Bob S.

Raider007 wrote:

[Raider_71]

Thanks guys!

[Anonymous]

I can see where this issue has the potential to cost a lot of people a lot of money.

There really should be some type of indicator when the dimension you are abouit to place is not projected.

My $.02

-Paul Cunningham

[Raider_71]

Yes I agree. The strange thing is that it still does it even if its a base view. Surely the default setting for all base views should be "Projected"???
At least I now know where to switch it over but its a matter of time before someone forgets to check it. So the only option is to use the registry option whereby all views are forced to be projected at all times.
Pieter

[Anonymous]

I think the way it works is okay, but there should be an indicator that the dim is true and not projected. Typically, you can tell by the angled dim text, but not always (this may be a style setting).

I think the registry setting just changes the default, rather than diabling true dim's altogether.

I'm just glad I didn't learn about this the hard way.

[Anonymous]

If the "base view" is NOT one of the six standard view orientations,
then dimensions are isometric unless you use the registry setting
mentioned previously to default all views to projected.

Raider007 wrote:
> Yes I agree. The strange thing is that it still does it even if its a base view. Surely the default setting for all base views should be "Projected"???
> At least I now know where to switch it over but its a matter of time before someone forgets to check it. So the only option is to use the registry option whereby all views are forced to be projected at all times.
> Pieter

[Anonymous]

Bob is correct: if the none of your origin planes from the model of your
views (base, projected or otherwise) are normal to the viewing direction
(parallel to your sheet), we tag the view as "isometric" and True,
model-calculated dimensions are created.

You can change the registry flag, or change that attribute from the view's
right-click menu.

One way you can differentiate true versus projected dims is just mouse over
the dimension. As we don't allow some of the drag-editing options for True
dimensions that we do for projected dimensions, the true dimensions only
have one set of green grip points on mouse-over where projected dimension
have three sets of grip points (see attached).

Of course, the best way to avoid this altogether is make sure your
assemblies are configured in such a way that they are aligned to the
assembly origin planes. If your processes don't really allow you to do
this, I'd recommend changing the registry setting.

Hope that helps clear things up.

--
Andrew Faix
Product Designer
Autodesk Inventor
---

"Bob S." wrote in message
news:5792976@discussion.autodesk.com...
If the "base view" is NOT one of the six standard view orientations,
then dimensions are isometric unless you use the registry setting
mentioned previously to default all views to projected.

Raider007 wrote:
> Yes I agree. The strange thing is that it still does it even if its a base
> view. Surely the default setting for all base views should be
> "Projected"???
> At least I now know where to switch it over but its a matter of time
> before someone forgets to check it. So the only option is to use the
> registry option whereby all views are forced to be projected at all times.
> Pieter

[Anonymous]

Hmm, not sure why the image didn't go w/ the last post. Here it is again...


"Andrew Faix (Autodesk)" wrote in message
news:5793075@discussion.autodesk.com...
Bob is correct: if the none of your origin planes from the model of your
views (base, projected or otherwise) are normal to the viewing direction
(parallel to your sheet), we tag the view as "isometric" and True,
model-calculated dimensions are created.

You can change the registry flag, or change that attribute from the view's
right-click menu.

One way you can differentiate true versus projected dims is just mouse over
the dimension. As we don't allow some of the drag-edit
ing options for True
dimensions that we do for projected dimensions, the true dimensions only
have one set of green grip points on mouse-over where projected dimension
have three sets of grip points (see attached).

Of course, the best way to avoid this altogether is make sure your
assemblies are configured in such a way that they are aligned to the
assembly origin planes. If your processes don't really allow you to do
this, I'd recommend changing the registry setting.


Hope that helps clear things up.

--
Andrew Faix
Product Designer
Autodesk Inventor
---

"Bob S." wrote in message
news:5792976@discussion.autodesk.com...
If the "base view" is NOT one of the six standard view orientations,
then dimensions are isometric unless you use the registry setting
mentioned previously to default all views to projected.

Raider007 wrote:
> Yes I agree. The strange thing is that it still does it even if its a base
> view. Surely the defaul
t setting for all base views should be
> "Projected"???
> At least I now know where to switch it over but its a matter of time
> before someone forgets to check it. So the only option is to use the
> registry option whereby all views are forced to be projected at all time

[Anonymous]

GRRRrrrr

3rd times a charm?



"Andrew Faix (Autodesk)" wrote in message
news:5793077@discussion.autodesk.com...
Hmm, not sure why the image didn't go w/ the last post. Here it is again.

[Anonymous]

"...tag the view as "isometric" and True,
model-calculated dimensions are created"

This is am imperceptible, yet critical change in behavior from previous versions.

There really needs to be a safety to prevent what happened to the original poster (and recommendations here don't fill the bill).

[Anonymous]

All three came thru fine on the web side

[Anonymous]

Well, I disagree that's it's imperceptible. If you apply constraints
appropriately, you'll never see this problem. You can verify the state of
the view by looking at your view's right-click menu.

There is a safety: it's the registry setting I detailed in the earlier post.


--
Andrew Faix
Product Designer
Autodesk Inventor
---
DIGITAL PROTOTYPING - Got it?


wrote in message news:5793083@discussion.autodesk.com...
"...tag the view as "isometric" and True,
model-calculated dimensions are created"

This is am imperceptible, yet critical change in behavior from previous
versions.

There really needs to be a safety to prevent what happened to the original
poster (and recommendations here don't fill the bill).

[Anonymous]

And if you use unorthodox views, coordinate systems, etc (and have been using them without problem for the past 11 releases), you'll never see this problem unitil the parts don't fit because the drawing was wrong due to the unexpected 'trueing' of the dimensions.

As I said previously, posts on this forum are not going to help most people until after the fact - not much of a safety.

I've been burned by Autodesk making stealth changes and it's no fun (MDT sp that changed view export-to-acad scale resulted in part being made 2x size) .

[Raider_71]

Hi Andrew,
Thanks for the tip but first of all I could not find that registry key you mentioned here. I did a search and found it in another location:
HKEY_USERS\S-1-5-21-292162120-3130509584-2557793563-1128\Software\Autodesk\Inventor\RegistryVersion12.0\Applets\DrawingLayout\Preferences\DrawingFormat
I changed it to 1 but everytime I start Inventor it changes back to 0. I then thought let me be clever and set the permissions so that it can not be changed but this even did not help. Inventor still inserts True dimensions.
Any idea what I can do?
I am running Windows Vista 32

Pieter

[Anonymous]

Well, first I'd double-check the reg key location again. I've attached a
screen shot of mine.

Also note that this setting only affects NEW views. Any views you've
already placed would have to be changed manually from the view's right-click
menu.


--
Andrew Faix
Product Designer
Autodesk Inventor



wrote in message news:5795177@discussion.autodesk.com...
Hi Andrew,
Thanks for the tip but first of all I could not find that registry key you
mentioned here. I did a search and found it in another location:
HKEY_USERS\S-1-5-21-292162120-3130509584-2557793563-1128\Software\Autodesk\Inventor\RegistryVersion12.0\Applets\DrawingLayout\Preferences\DrawingFormat
I changed it to 1 but everytime I start Inventor it changes back to 0. I
then thought let me be clever and set the permissions so that it can not be
changed but this even did not help. Inventor still inserts True dimensions.
Any idea what I can do?
I am running Windows Vista 32

Pieter

[Raider_71]

Hi Andrew,

I have verified this on Windows XP pro. The registry key is in the location you said and I can force the dimensions to be projected. However on Windows Vista this is not the case. I am running Vista 32 on my PC and that registry key does not change the way inventor handles dimensions.

Pieter

[Anonymous]

Hi Pieter,

Sorry you're having problems.

Vista heh? Hmmm, I'm going to have to ask someone in QA to get involved.

Sorry, I don't have anything now, either myself or someone else will post
back here once/if we can get the problem verified.


--
Andrew Faix
Product Designer
Autodesk Inventor



wrote in message news:5796453@discussion.autodesk.com...
Hi Andrew,

I have verified this on Windows XP pro. The registry key is in the location
you said and I can force the dimensions to be projected. However on Windows
Vista this is not the case. I am running Vista 32 on my PC and that registry
key does not change the way inventor handles dimensions.

Pieter

[gabriel.lengyel]

Hi Pieter,

I tried to change mentioned registry setting and it worked under my 32bit Vista. Please ensure that Inventor is not running when editing the registry.

Do you still see the problem?

Regards,

Gabriel.