Inventor General Discussion

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Member
rdenning
Posts: 3
Registered: ‎11-25-2002
Message 1 of 5 (314 Views)

Dimensioning Isometric Drawing File...

314 Views, 4 Replies
11-25-2002 06:14 AM
When I dimension an isometric Drawing file (*.idw) in Inventor 5.0, the dimension is not accurate. Why is this?

If I dimension a front, right, or top view the dimensions are accurate. But once I revert to the iso, they aren't. This is a bit frustrating, so any help would be appreciated greatly.

Thank you.
*Maas, Karl
Message 2 of 5 (314 Views)

Re: Dimensioning Isometric Drawing File...

11-25-2002 09:13 PM in reply to: rdenning
its a bug. We should ask in the R6 group if it's
fixed there.


--
K

 

 


style="PADDING-RIGHT: 0px; PADDING-LEFT: 5px; MARGIN-LEFT: 5px; BORDER-LEFT: #000000 2px solid; MARGIN-RIGHT: 0px">
When
I dimension an isometric Drawing file (*.idw) in Inventor 5.0, the dimension
is not accurate. Why is this?

If I dimension a front, right, or top view the dimensions are accurate. But
once I revert to the iso, they aren't. This is a bit frustrating, so any help
would be appreciated greatly.

Thank you.

Member
rdenning
Posts: 3
Registered: ‎11-25-2002
Message 3 of 5 (314 Views)

Re:

11-25-2002 09:41 PM in reply to: rdenning
Do you know if there is an update that can be downloaded to fix this? If not, would they even bother with one, if R6 is out? Thanks......
*W, Tim
Message 4 of 5 (314 Views)

Re:

11-25-2002 10:58 PM in reply to: rdenning
The short answer is that isometrics come in scaled because of "proper
drafting standards".
I've copied and pasted a message from the "autodesk.inventor.support"
newsgroup (read only now, but still very helpful) dated Oct 28, 2002 that
answers your question more fully.
All lines from that post start with "> ".
Now, to make the dimensions correct... you can't. I haven't found a "scale
factor" variable in the dimension style. Even if you scale your iso view by
about 1.225 (to make it actual 1:1), your dimensions are automatically
scaled by this factor when dimensioning the view. Thus, they read the same
number. The only work around that I can think of is to export your
scaled-up iso view to AutoCAD and dimension it there.
If anyone else knows a better way, please advise!
Oh, I did just think of one... use a derived part... scale it up by about
1.225... then insert it into the drawing at 1:1. I haven't tried it yet,
but I *think* it will work.

Hope this helps...
Tim

> ----- Original Message -----
> From: "Howard Delano"
> Newsgroups: autodesk.inventor.support
> Sent: Monday, October 28, 2002 1:33 PM
> Subject: Re: Isometric drawing scale


> Good info Bill. Picture showing where this comes from can be found at the
link below. Because the isometric corners are drawn at 120 degrees, not 90,
there is a difference in length from true value. I think that CAD systems
use an angle slightly different than 120 because it is "correct" and they
can. It was just easier to draw it at 120 by manual means in the old days.
Thus the difference between 81.6 and 84.6%.
>
> http://www.globalspec.com/RefLibrary/CDS/iso1.gif
>
>
> --
> Thanks,
>
> Howard Delano
> Design Engineer
> Stainless Design Concepts
> A Division of CVD Equipment Corporation
> 1117 Kings Highway
> Saugerties, NY 12477
> Phone: (845) 246-3631 (ext. 38)
> Fax: (845) 246-1595
> E-mail: hdelano@stainlessdesign.com
> "Bill Bogan" wrote in message news:92C7B55E152DCFD
5D37CFE541A6EC6CF@in.WebX.maYIadrTaRb...
> My only guess about why you are asking is that you have exported an
isometric view to ACAD and dimensioned it.
> Is that correct? If so, please note this fact about isometric views....
>
> True isometric views have lines that are approx 82% (0.816) of the
actual length.
> The resulting view can be scaled to 1:1 if you want. But I assume that
that is why it starts out at approximately the size it does.
> This value (82%) was obtained from the following: "Technical Drawing" by
Geisecke | Mitchell | Spencer | Hill
> Fifth edition (old)
>
> --
> Bill Bogan
> "Wogz" wrote in message
news:f11cc64.-1@WebX.maYIadrTaRb...
> hi all,
> I've already asked this, but no responces, so I'm posting it again..
>
> In Inv and MDT (pretty much all versions), why is it that a 1:1
Isometric isn't 1:1? The Iso view is usually scaled by 0.846%. Does anyone
know? Has anyone wondered this?
>
> Previous post is about oct 24, 2k2..
>

"rdenning" wrote in message
news:f127458.1@WebX.maYIadrTaRb...
Do you know if there is an update that can be downloaded to fix this? If
not, would they even bother with one, if R6 is out? Thanks......
Distinguished Contributor
JDMATHER
Posts: 4,994
Registered: ‎12-12-2003
Message 5 of 5 (314 Views)

Re: Dimensioning Isometric Drawing File...

11-26-2002 12:57 AM in reply to: rdenning
Start a new drawing and bring in the part as a derived part with a scale of 1.224744873

Now Iso will give correct dimensions in my test, but how can the extension lines be obliqued?

J.D.
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