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BETTER METHOD FOR ALIGNED IDW DIMENSIONS

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Message 1 of 10
brendan.henderson
2189 Views, 9 Replies

BETTER METHOD FOR ALIGNED IDW DIMENSIONS

I know there are work arounds (view sketches, rotated views) for aligned dimensions, but it simply needs to be done better. Even if it became Autocad like where you can align the UCS with a line and apply the dimension as needed and then align the UCS with World again. All I need is controls to place a dim between the 2 holes with the dim aligned to the lien indicated. Comments and solutions appreciated.

 

ALIGNED_PARALLEL_DIM.png

Brendan Henderson
CAD Manager


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Inventor 2016 PDSU Build 236, Release 2016.2.2, Vault Professional 2016 Update 1, Win 7 64 bit


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Message 2 of 10

In these cases i help myself with sketches.

 

 

q.gif

Admaiora
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Message 3 of 10

Thanks for your input and the video. I know I can do this, but I consider it too much work, too clumsy and a work around. I'll post this to the IdeaStation also.

 

Edit: here is the link to the IdeaStation post.

Brendan Henderson
CAD Manager


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Inventor 2016 PDSU Build 236, Release 2016.2.2, Vault Professional 2016 Update 1, Win 7 64 bit


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Message 4 of 10

Another method you can use.

 

Apply a CHAIN SET dimension.

Select the line you wish to align to FIRST, then the holes to be dimensioned.

You should end up with something like this.

Aligned - Select.JPG

 

Now hover over the end of the line and RMB and select DELETE member.

Do this for both ends of the line and you should end up with just a hole to hole dimension aligned to the desired line like so.

Aligned - Final.JPG

Mike Patchus - Lancaster SC

Inventor 2025 Beta


Alienware m17, Intel(R) Core(TM) i9-10980HK CPU @ 2.40GHz 3.10 GHz, Win 11, 64gb RAM, NVIDIA GeForce RTX 2080 Super

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Message 5 of 10
admaiora
in reply to: mpatchus

Nice Mpatchus!

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Message 6 of 10

Align.PNGAnother option might be right click on your center marks and edit/Align to Edge, Pick the line you want.

This will rotate youe center marks to the edge. Now just use the std dimension tool.

Douglas DuPont
Inventor 2016 Pro, Vault 2016 Pro
Quadro M4000
Windows 10 64 Bit
Message 7 of 10
mpatchus
in reply to: Doug_DuPont

Good point Doug. 

 

Some folks don't like seeing the center marks orientated any way rather than horz/vert, so once you have placed the aligned dimension, you can realign your center marks back to normal.

The aligned dimension will "hold" even though the marks have been realigned.

Mike Patchus - Lancaster SC

Inventor 2025 Beta


Alienware m17, Intel(R) Core(TM) i9-10980HK CPU @ 2.40GHz 3.10 GHz, Win 11, 64gb RAM, NVIDIA GeForce RTX 2080 Super

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Message 8 of 10

When on applies constraints one can 'rub' an existing line to tell IV that you want to constrain to that line.

 

What would be nice (HINT, AUTODESK) here would be a similar workflow in that one would pick the two endpoints of the aligned dimension, rub on a line to which you want the dimension to parallel, then place the dimension.

IV 2013 Product Design Suite 64 Bit
Win 7 64 bit
Message 9 of 10

Thanks Mike.Rather un-intuitive and requires a considerable amount of make/delete but could be usable.

Brendan Henderson
CAD Manager


New Blog | Old Blog | Google+ | Twitter


Inventor 2016 PDSU Build 236, Release 2016.2.2, Vault Professional 2016 Update 1, Win 7 64 bit


Please use "Accept as Solution" & give "Kudos" if this response helped you.

Message 10 of 10

Thanks Doug. Also usable like Mikes solution, but I agree with Mike. The centre marks need to be rotated back to vertical.

Brendan Henderson
CAD Manager


New Blog | Old Blog | Google+ | Twitter


Inventor 2016 PDSU Build 236, Release 2016.2.2, Vault Professional 2016 Update 1, Win 7 64 bit


Please use "Accept as Solution" & give "Kudos" if this response helped you.

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