Problem with dimensions in IDW

[martin_halacek]

I face problem with dims in IDW. Attached picture demonstrates the issue. Dim is different from the same dim in parent view of projected view with a break view . Parent view is very slightly angled (I mean top line is not 100% horizontal) , but that can´t make such big difference like 2509 vs. 241. Naturally dim is not manually overwritten. I have Inventor 2018 R2 build 227 (latest) and I have never noticed anything like that in Inventor during last 10 years or so. May be the problem is somehow related to opening IDWs created in older Inventor versions or IDW migration , because IDW was made in 2015 . Unfortunately, we have some parts already produced with wrong size.

[mdavis22569]

Can you share the file ... that would probably be the fastest way ...

[martin_halacek]

No problem. I attached files.

[mdavis22569]

First think I noticed:

2nd think I noticed

All of the views are on an angle ...

So it goes on an multiple angles ... so you'll never get it just right. You'd need points to pick from.... it has a radius on the end edges... you'll need to turn on the hidden lines too

[SBix26]

Strange. 

• The view with the bad dimension doesn't show the broken view indicators as it should. 
• If I place a new projected view just like it, it behaves as you would expect.  
• If I change the General Dimension Type of the bad view to True, a new dimension is placed correctly.

This looks like one for the Autodesk QA folks to sort out.  @johnsonshiue, are you available?

Sam B

Inventor Professional 2018.2
Vault Workgroup 2018.0
Windows 7 Enterprise 64-bit, SP1

[martin_halacek]

Thank guys for your effort.

I also noticed that zig-zag symbol is missing in the bottom view. Strange thing is , that when I move the borders of the break view in the top view , dim at the bottom changes. I suppose that it should stay the same. I don´t understand what happens there.

[SBix26]

That dimension in the bottom view seems to be giving the actual measurement on the drawing sheet, not taking into account the missing material.  If I start a view sketch and place a line with that dimension, it matches perfectly:

Sam B

Inventor Professional 2018.2
Vault Workgroup 2018.0
Windows 7 Enterprise 64-bit, SP1

[mdavis22569]

I did change my view orientation too ... so It was true.

[johnsonshiue]

Hi! I took a look at this case. I think I got better understanding now. There are a few things with this dataset.

1) The assembly has interference. Look at how V-70-080753-1:1 and V-70-060427:4 are constrained. Turn on Shaded Edge display. You will see the two parts collide. The way they were constrained are not right. If you measure the two side faces, there is a 0.44 deg.

2) The inconsistent dimensions have something to do with the Auxiliary view. Do you notice that the Break view symbol does not carry over to the Aux view? It is because Aux views may not be orthogonal and the dimension may not be the same as orthogonal views. If the view is projected view, the Break view symbol will carry over and the dimension will be in sync.

Many thanks!