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Dimension Beveled Tube Ends

12 REPLIES 12
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Message 1 of 13
mies07
1101 Views, 12 Replies

Dimension Beveled Tube Ends

Can someone please tell me how to create the dimension shown in an idw? Thanks.

Bevel Dim.jpg

12 REPLIES 12
Message 2 of 13
alessandro.gasso
in reply to: mies07

I hope you can find useful the video attached.

 

Kind regards,

Alessandro



Alessandro Gasso
Fusion 360 – Simulation/Generative Design Adoption Specialist
Autodesk, Inc.
Message 3 of 13
Doug_DuPont
in reply to: mies07

You can put a horiz dimension from the 2 points and then right click on the dimension and select align to edge and pick the angled line.

Douglas DuPont
Inventor 2016 Pro, Vault 2016 Pro
Quadro M4000
Windows 10 64 Bit
Message 4 of 13
mies07
in reply to: Doug_DuPont

Align to edge? I get no such option when right clicking the dim... perhaps a screen shot?

Message 5 of 13
Doug_DuPont
in reply to: mies07

Your right, I had confused that with the center line align to edge. Sorry.

Sounds like a good wish list item.

Douglas DuPont
Inventor 2016 Pro, Vault 2016 Pro
Quadro M4000
Windows 10 64 Bit
Message 6 of 13
IgorMir
in reply to: alessandro.gasso

That's just brilliant! Sorry, I can't thank you for your effort. Your video is just a poor workaround to the problem existed in Inventor from the day one. What if you have to dimension more then one trace like that? You guys should hook up for a lunch with your friends at AutoCAD team and find out in details how Align UCS tool works in AutoCAD. Then introduce that very tool in Inventor drawing environment. That is a solution to the dimensioning problem discussed, not the auxiliary sketch workaround.

Best Regards,

Igor.

 


@alessandro.gasso wrote:

I hope you can find useful the video attached.

 

Kind regards,

Alessandro

Web: www.meqc.com.au
Message 7 of 13
ianmacleanllc
in reply to: IgorMir

this one gets me as well.... i gues they have never worked on the shop floor.

my saw operator is always asking for "long point to long point" 

 

Message 9 of 13
Martin_Goodland
in reply to: mies07

You can add workpoints in the part model, then bring these points into the drawing, align them to the desired edge and dimension between them. I find this neater than adding sketches to the drawing views as I have had instances where the sketches in the .idw don't update and the dimensions then become incorrect.

 

Still not as neat as an 'align to edge' option though.......

 

Regards

 

Martin

Inventor 2023
Message 10 of 13
julesgf
in reply to: mies07

I have noticed that (at least in recent versions) you can use the "chain" dimension type (not chain set) to achieve this.

place the dimension by hitting chain -> click on the line parallel to the dimension to be placed -> place as an aligned dimension -> RMB create -> drag one end of the dimension out to the long end of the bevel.

Dimension remains aligned to the first selected line (unlike a general dimension that will become a point to point when dragged to bevel end)

See attached (pretty rough quality Smiley Happy) video)...

Drove me mad till I discovered it.

 

Cheers

Message 11 of 13
julesgf
in reply to: julesgf

Don’t know why I wound up with 2 videos, they'll both be the same.

it complained that the 1400k was too big then accepted the 1200 and posted both!

Message 12 of 13
SBix26
in reply to: julesgf

This is a great tip (or is that a workaround?!).  However, you have to be careful- a dimension placed that way does not maintain its alignment to that edge, so a model change that causes the angle of the edge to change will make that dimension useless.  No problem, if the change is big enough to notice; possibly a serious problem if it isn't.

Message 13 of 13
mies07
in reply to: mies07

Thank you all.

I discovered you can do the same thing as was in the video with a base line dimension, but you end up having to erase a few of the base line dimensions to leave the one you want. The key is where to hover your mouse before creating the dim.

Of course, I can do this in AutoCAD (surprisingly enough, also an Autodesk product) with a rotated dimension, and it doesn't require nearly as much hand-eye co-ordination. It's also documented in Acad.

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