Inventor Contstrain Section Line So Hole Location Moves Associate To Update

[domcm]

I am trying to create an associative section line on a drawing in Inventor 2018 so that when a hole location moves, the section line moves with it. Is this possible? I added a coincident constraint aligning the section line with the datum point locating the hole, but when I change the hole location, the section line is not moving with it. Am I doing something wrong? See attached video and Inventor files.

kelly.young has edited your subject line for clarity: Associative Section Line?

[SBix26]

Right click on the section line and select Edit.  This allows you to edit the section definition as a sketch.  Use Project Geometry to project the hole, and then constrain the section definition line to the hole center.  Exit sketch, and now the section line is constrained to the hole.

Hope this helps,

Sam B

Inventor Professional 2018.2
Windows 7 SP1

[domcm]

@SBix26 Thanks, I actually tried that but could not get it to work. If you open the drawing, you will see that the section line has a coincident constraint applied to the datum point locating the hole centerline (I could not get a hole center snap when I projected the hole outline). Problem is, when I move the hole, the section line does not move with it. You will see in the video that when I edit the section line and move it a bit, the section line snaps back to the hole centerline - but only when I edit the section line.

[johnsonshiue · Accepted solution]

Hi! Indeed, I am able to reproduce the behavior using the files you attached. It seems like a bug or a limitation that the projected workpoint in the drawing does not update automatically. If you edit the section sketch and drag the line a bit, the vertical section line will snap.

The interesting thing is that if you do the following, the section line will update correctly.

1) Edit the section sketch.

2) Show all constraints.

3) Delete the project constraint -> Finish the sketch

4) Include Work Plane2 in the drawing,

5) Edit the section sketch.

6) Create a colinear constraint between the section line and the projected sketch -> Finish the sketch.

Many thanks!

[SBix26]

Hmm, I didn't notice the existing constraint when I opened the drawing; I projected the hole outline, then constrained the midpoint of the sketch line to the center of the hole... which turns out to be your already projected point.  The projected hole does not create a center point, presumably due to the fact that the actual hole edge is a spline.

So, the question is: why does it work when the midpoint of the sketch line is constrained to the projected point, but doesn't when just the line is similarly constrained?

Sam B

Inventor Professional 2018.2
Windows 7 SP1

[johnsonshiue]

Hi Sam,

This one looks more like a bug to me. I don't have a good explanation. It is possible a limitation also. I will work with the project team to understand it better.

Many thanks!

[kelly.young · Accepted solution]

@domcm to add to what @johnsonshiue states, another way you could do it:

• Edit the Section Line Sketch
• Project Geometry of the circle
• Create a Two Point Center Rectangle that encompasses the circle
• Make Tangent Constraints all around.
• This will give you the center point to constrain the midpoint of the section line to.
• You can do this easily in the sketch where the section line is defined and shouldn't be too much work.  

This looks like something that is working just not updating with the part. The development team has been notified. Hope that helps!