Parallel lines dimension value is 180° instead of linear value

[ToddPig]

Recently I started getting a value of 180.00° when trying to dimension two parallel lines in a sketch.  I get around this by selecting one line, and then an endpoint on the other line, but sometimes this requires the extra step of zooming to the endpoint of the line.  Is there a setting that I could've accidentally changed?

Thanks in advance,

Todd

[JDMather]

Can you attach file here that exhibits this behavior?

If you set to show all decimal places - is it really parallel?

[ToddPig]

JD,

Unfortunately, I can't attach this file, as I am working in an assembly, but the next time I get this in a sketch, I will attach the file(s). The main reason for this post, was this only RECENTLY starting happening. Maybe in the last 2 or 3 weeks. I have even had it happen with creating a vertical line, then using the offset command to make a line parallel. then later on trying to dimension the distance between the lines only to have it show an angle dimension instead of a linear value.

[ToddPig]

5 DECIMAL PLACES, STILL GIVES ANGLE DIMENSION INSTEAD OF LINEAR DISTANCE.

WHEN I ADD THIS SAME DIMENSION IS A DRAWING, IT SHOWS AS A LINEAR VALUE.

CONFUSED.

TODD

[SBix26]

Been using Inventor since 2002, and the only time I've ever seen this happen is when the elements are actually out of parallel.  Use the Measure Angle command, and be sure that the Precision is set to All Decimals-- does it read 180° (or 0°), or does it have a few decimals showing out at the 8th or 9th place?

Sam B

Inventor Professional 2017 R2
Vault Basic 2017.0.1
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

[Nauld1]

I'm having this issue right now, lines are definitely parallel. But when I try to add a linear dimension in the sketch all I get is an angled dimension. 

[SBix26]

Works for me (Inventor 2021.4.1):

Maybe you could capture a Screencast video of you placing that dimension?

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Sam B

Inventor Pro 2023.0.1 | Windows 10 Home 21H2

[Nauld1]

That's not the right one, you need to try one of the bottom 2

[Nauld1]

And as I said the problem is only IN SKETCH not on the drawing itself

[Nauld1]

I wanted to add the dimension between the drawn rectangle and the projected line circled.

[Nauld1]

just to show that they definitely have 0 degrees between those 2 lines.

[SBix26]

I think this qualifies as a bug in Inventor; if you measure from the sketched geometry to the projected line, it shows an angular dimension of zero, to the maximum decimal places.  If you measure from the sketched geometry to the two endpoints of the projected line, they are not identical in the last three decimal places, indicating a very slight angle exists, but definitely beyond any reasonable precision.

The fix is pretty simple, though-- delete the Horizontal constraints on the sketched lines, and instead make them parallel to the projected line(s).  Then they dimension properly.

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Sam B

Inventor Pro 2023.0.1 | Windows 10 Home 21H2

[Rob_Windsor]

I have found that the rectangles are slightly at an angle... to the extent that you cannot see it, even to the maximum decimal places. 

I definitely had the same issue of only getting angle dimensions.  If you look at the sketch, the rectangles are "Fixed" in place.  I removed the fixed constraints and added a horizontal constraint and it worked perfectly.  I can only assume that the rectangles were not added with the rectangle tool in Inventors sketch environment.  Inventor is not recognizing the inserted geometry as perfectly horizontal. 

Just to go a bit deeper, I dimensioned to the end points of the rectangles and got two different dimensions:  6.0000002 in and 6.0000001 in.  It is not horizontal.  I hope this helps.