Dimensions on angled lines in drawing

[Anonymous]

I am having trouble with dimensions of angled features in the drawing.  The dimensions are not parallel to the angled lines, keeps snapping to the end points of the lines.  Any suggestions for a fix or work around?  Attached are photos of what I am having trouble with.

[SaeedHamza]

Hi,

Check this screencast please

https://knowledge.autodesk.com/community/screencast/83f4d66d-1229-4c33-b3a8-29a1384e1c9d

Regards, Saeed

[Anonymous]

Below is a screencast of what I am having issues.  Please let me know if there is a work around/fix.

[Anonymous]

Below is the second item I am having issues with.

[cmiller66]

Hi Kenneth,

For the first issue, when you hover over that first line segment and see the dimension preview appear, click to select the line.  Now hover over the parallel edge and you'll see the dimension flip to aligned.  Click to select that 2nd line and drag the dimension out and place it.

The second case isn't so straightforward, because we don't currently have a way to select that first point then specify Perpendicular to that slot's edge. There also isn't a 2nd reference edge (like in case 1) to dimension against.  We can create aligned dimensions line-line, not point-line.  We do have plans to allow snap overrides, in this case it seems like the dimension you want is from that initial point perpendicular to the edge.

The only workaround that's coming to mind is creating a detail view of that slot, then rotating the detail view so the dim can be created, even then I'm not sure you're going to get exactly what you're going for.  Would you be able to send me this design (f3d)?  I'd like to try a few things if possible.  Please send to christopher.miller@autodesk.com.

Thanks,

Chris

[danolson1]

I'm having the same problem.  I have a drawing and I would like to draw a dimension between a line and a point, perpendicular to the line.  I used the workaround of making a detail view and rotating it, but this is not an ideal solution.

Here is a link to the drawing I'm working with.  The problem dimensions are the between the 1" hole (1 1/2" in one direction and 2" in the other direction)

http://a360.co/2rKytVn

-Dan

[cmiller66]

Hi Dan,

Thank you for sharing your design and drawing. We still have this feature on our roadmap and are definitely aware of the requirement to place a dimension this way (point to a line).

In the meantime for this case I was able to dimension the view by using a center mark.  

1.  Center mark > Apply to the hole

2.  Select the center mark > Rotate it 45 degrees

3.  Select the center mark > Using the arrow grip stretch it "down" towards the endpoint indicated

You can now use an aligned dimension from endpoint to endpoint to place the 1 1/2" dimension

4. For the 2" dimension, use the dimension tool and select the centermark line (not the endpoint) then the angled 45 degree edge (you'll see the dimension preview if you have the edge selected).

It's a few extra steps, as is the rotated detail view, but it will let you dimension the view in place.

Thanks,
Chris

[danolson1]

Thanks.  That works.  I didn't know you could rotate center marks.