Off-Sheet Center Point - Proper Way to Dim

[Anonymous]

What is the proper way to dim a radius center point
that is off-sheet, drawing view sketch with manual over-ride dims?

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3.2
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SpacePilot Rel V: 3.6.11 Dvr V: 6.6.4 Firmware 3.12
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8.5

[Anonymous]

Blair, I don't know if this is "proper", but I think I remember a user posting a tip that you can add a break in the view and adjust so that the centerpoint is on the paper.



Nevermind, I couldn't get it to work in 2009. Maybe there was a trick I'm forgetting...

Edited by: Josh_Petitt on Apr 14, 2009 4:23 PM

[Anonymous]

That was the first thing I tried, you get a
"Invalid Material Removal" or to that effect

--
IV2010pro-suite
Dell 670 dual Xeon - 3.2
3gb memory,
SCSI320-15k rpm
XP-Pro, sp3
Quadro FX3400: Driver: 182.08
Direct3D
SpacePilot Rel V: 3.6.11 Dvr V: 6.6.4 Firmware 3.12
AVG 8.5

style="PADDING-RIGHT: 0px; PADDING-LEFT: 5px; MARGIN-LEFT: 5px; BORDER-LEFT: #000000 2px solid; MARGIN-RIGHT: 0px">

<Josh_Petitt> wrote in message
href="news:[email protected]">news:[email protected]...

Blair, I don't know if this is "proper", but I think I remember
a user posting a tip that you can add a break in the view and adjust so that
the centerpoint is on the paper.



Nevermind, I couldn't get it
to work in 2009. Maybe there was a trick I'm forgetting...

Edited by:
Josh_Petitt on Apr 14, 2009 4:23 PM

[Anonymous]

yeah same here. I swear I remember a post where someone else was discussing this, but I unfortunately couldn't find it w/ the search.

[Anonymous]

echo

[Anonymous]

There must be something, how would you DIM a small
part that has a large radius where you need to locate the center point of the
radius. Very odd....

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IV2010pro-suite
Dell 670 dual Xeon - 3.2
3gb memory,
SCSI320-15k rpm
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Quadro FX3400: Driver: 182.08
Direct3D
SpacePilot Rel V: 3.6.11 Dvr V: 6.6.4 Firmware 3.12
AVG 8.5

style="PADDING-RIGHT: 0px; PADDING-LEFT: 5px; MARGIN-LEFT: 5px; BORDER-LEFT: #000000 2px solid; MARGIN-RIGHT: 0px">

<Josh_Petitt> wrote in message
href="news:[email protected]">news:[email protected]...

echo

[dan_inv09]

Is this the one?

http://discussion.autodesk.com/forums/thread.jspa?messageID=5803728軐

[Anonymous]

that's the one, thanks Dan!

[pauldoubet]

Please see the attached file for the ASME Y14.5 explanation of how to do this.

Hope this helps, Paul

[Anonymous]

Thanks, that was what I was thinking that I might
have to do. I would be nice to place the dimensions, then do a "Broken View" to
bring them into a respectable location in relation to the drawing
view-scale.

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Direct3D
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AVG 8.5

style="PADDING-RIGHT: 0px; PADDING-LEFT: 5px; MARGIN-LEFT: 5px; BORDER-LEFT: #000000 2px solid; MARGIN-RIGHT: 0px">

<Josh_Petitt> wrote in message
href="news:[email protected]">news:[email protected]...

that's
the one, thanks Dan!

[Anonymous]

> {quote:title=pauldoubet wrote:}{quote}
> Please see the attached file for the ASME Y14.5 explanation of how to do this.
>
> Hope this helps, Paul

That's all well and good, but Inventor doesn't support it (or it's not easily discoverable).

[SBix26]

As you can see from the old thread that Dan found, it has been a problem for many years with absolutely no response from Autodesk. It's also been in the AUGI Wishlist a number of times, but doesn't get enough votes to make it to the top ten list.



I'm sure it's not a trivial task to make a good foreshortened radius/displaced centers tool, but we really don't have an adequate way to produce good drawings of such parts at this time with Inventor.



Sam

[Anonymous]

"absolutely no response from Autodesk"



That's not true. A few versions back, you could move the ceter point onto the sheet by using 'broken view' command to break the empty space. But after you did so, you couldn't edit or delete the break.

Autodesk 'fixed' this in recent versions by not allowing you to break empty space. 😛



The ability to create each type of dimension shown in the ANSI standards (without workarounds) really shouldn't need to go onto a wish list.



-Paul Cunningham

[Anonymous]

The fact that the dim type in question doesn't currently exist makes it an "enhancement" in Autodesk's eyes. It's only a "bug" if they currently offer it, but something in the process is wrong or broken.

People need to simply keep asking for it. Don't expect it though ... that way you'll be surprised when (if) it shows up.

[pauldoubet]

Well I may have misunderstood the original question. It seems you are looking for some toolbar button or option to automate this process. It does not exist I agree, however the tools to solve this problem do exist.

1. Create the foreshortened radius dimension.
2. Create a sketch in the required view consisting of two crossing line segments whose midpoints are coincident for a center mark.
3. Change the style of those two segments to the Centerline style.
4. Add sketch dimensions to adjust location and size of the line segments.
5. Finish the sketch.
6. Add dimensions for X and Y to the center mark and drag the radius dimension to align with the center mark you just sketched and dimensioned.
7. Edit dimension to hide model value.
8. Edit text and insert model parameter for the correct X and Y values from the part file.
9. Create a symbol for the double arrow head.
10. Insert the symbol were needed.

Do you really think Autodesk should give this a very high priority based on the few times it is required?

I don't care if they ever add a toolbar button or option to do this, I feel there is already a solution.

Good Luck, Paul Edited by: pauldoubet on Apr 18, 2009 7:37 AM

[Anonymous]

"...I feel there is already a solution."



Careful. Someone from Autodesk might read this, miss the sarcasm, and think you're actually serious.



-Paul Cunningham

[Anonymous]

This solution results in a non-parametric dimension.  It's a work around and not a soluition.  If available, I would use this functionality on a daily basis.

[Anonymous]

Did this ever get resolved?  Is creating a sketch the only solution?

[SBix26 · Accepted solution]

Here is one Idea posted to the Inventor Ideas forum, and here's another one.  I thought that I had posted one, but I can't find it.

My current workaround is to create a very tiny feature in the model at the radius center.  This provides actual model geometry so that you can break the view.  Linear dimensions to the center mark are associated properly, and show the break mark, as they should.  Unfortunately, radial dimensions don't adjust properly, though the value is correct.  This is as close as we can currently get to ANSI Y14.5 compliance, I believe, while still retaining associative dimensions.

One thing I haven't tried is to make the tiny center geometry a separate solid, and whether a view rep with this solid invisible would still allow the broken view functionality (either before or after placement & Break operation).

Sam B

Inventor Professional 2017.3.1
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Inventor Certified Professional

[Anonymous]

Thanks.  I hate to make that as a solution, because I do not want AutoDesk to think it was a done deal.  Kudos instead....