Align drawing views to the bottom (not the centre) of view

[Anonymous]

Hello, 

Does anyone know any way to align 2 or more drawing views to the bottom of the view not the middle of the view?

See the screenshot below of what I am trying to achieve:

I have just roughly positioned these 2 drawing views by eye. I want them to be exactly aligned along the bottom so that the castors would all sit along a straight line. 

Thanks for any help, 

Finn

[Mark.Lancaster]

@Anonymous

If you right mouse click on a given view and select alignment from the contextual menu.

[Cadmanto]

The alignment command does not give you the option to choose an edge to align to.

Take a look at this thread.  It speaks to what you are looking for and has a link to an idea to enhance the alignment command to do what you are asking.

https://forums.autodesk.com/t5/inventor-forum/view-alignment/td-p/6209545

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2018

[Cris-Ideas · Accepted solution]

Hi,

If this is the same assembly you can get that but with a workaround

Have two views of the assembly in the same POS REP.

Change view setting from centred to fixed

Brake out alignment.

Change POS REP in the view you want.

Cris.

[Anonymous]

Problem solved

As it was the same assembly but different positional representations that I wanted to line up I could use the workaround that Cris suggested. 

Cheers mate, appreciate it. 

I have also added to that thread so hopefully it may get changed in the future. I am surprised that there aren't more users with this problem. 

[Cris-Ideas]

There are but Autodesk only does what it thinks is needed and fixing bugs and removing stupid limitations is not high on their list.

So people just quite trying. and either leave or live with it.

Workaround I gave, you can also use in other situations but this requires additional tricks if you want to align different assemblies or parts.

Cris

[rayessle · Accepted solution]

You could try adding and running this ilogic rule.

1. pick the view you want to keep in position.

2. pick the view you want to align. the view will move in the vertical direction to align both bottom edges of the views.

oView1=ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, "Select the a view to retrieve position of")

pt1 = oView1.Position
'MsgBox("X: " & pt1.X & vbLf & "Y: " & pt1.Y)
ht1= oView1.Height

oView2 = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, "Select the a view to align position of")

pt2 = oView2.Position
ht2 = oView2.height

ActiveSheet.View(oView2.name).SetCenter(pt2.X * 10, (pt1.Y - (ht1/2) + (ht2/2))*10)

[Anonymous]

Thanks a lot Ray, that tool works perfectly!

Finn

[SER4]

I'm running 2019.  Does this iLogic work for anyone else?

The 2nd drawing view selected seems to become hidden (still an entry in the browser though).

[rayessle]

Are you using this on an 'imperial' ie not metric drawing sheet? Just tried it and it works on the metric drawing sheets in 2020 but not the imperial ones.? It does actually move the view but puts it off the drawing sheet (outside the border) Will try to work out why.

[rayessle]

Changing the 10 factor to 10/25.4 seems to work.

oView1=ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, "Select the a view to retrieve position of")

pt1 = oView1.Position
'MsgBox("X: " & pt1.X & vbLf & "Y: " & pt1.Y)
ht1= oView1.Height

oView2 = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, "Select the a view to align position of")

pt2 = oView2.Position
ht2 = oView2.height

ActiveSheet.View(oView2.name).SetCenter(pt2.X * 10/25.4, (pt1.Y - (ht1/2) + (ht2/2))*10/25.4)

[SER4]

Not to discredit your work, @rayessle, but I have found the following forum thread in which you can align views by lines (e.g. sketch lines), which is very helpful for more than just vertical & horizontal (e.g. triple axisymmetric).

https://forums.autodesk.com/t5/inventor-forum/aligning-views-to-a-line/td-p/7186354

[kadscad]

SOME ONE THAT KNOW HOW TO CODE NEEDS TO FIX THIS

[johnsonshiue]

Hi! Please see my latest reply to your message.

https://forums.autodesk.com/t5/inventor-forum/view-alignment/m-p/11800047/highlight/false#M889925

Many thanks!