Ordinate Dimension to an Intersection

[Alan Coons]

I can put a regular dimension to an intersection, but when I rmb I do not have the intersection option when placing an ordinate dimension. Is there another way to go about putting an ordinate dimension to an intersection?

[Anonymous]

Hi Alan,

Is the intersection a virtual intersection?

Thanks,

Lati Mu
Inventor QA
Autodesk

[Alan Coons]

It is the intersection of two centerlines.

[Anonymous]

Could you please post a picture ?

Thanks,

Lati Mu
Inventor QA
Autodesk

[Alan Coons]

Here is a pic of what I get when I try to add an ordinate dimension to the intersection of two centerlines. I am trying to place at the intersection of the horizontal line and the line approximately 60 degrees to it.

[Anonymous]

Hi Alan,

Adding an ordinate dimension member on an intersection point between
centerlines is not supported in IV10. I can log a wish list item and
consider this in a future release.

Thanks for the feedback!

Lati

[ToH]

A wokaround could be to place a sketch in the drawing view, project some relevant geometry, and finally draw and constrain a small line to the position you want for the dimension.

(I know, this is not what you asked for, but it might solve the problem)

Torbjørn

[CelticDesignServices]

Resurrecting an old post here but the last post (the work around) is a bit unacceptable as far as I'm concerned.

I've got an example where we are dimensioning from a hard edge to the intersection of a hard edge and a centerline. How do we add an ordinate dimension to this situation? Again, adding a sketch for this is not acceptable in my book.

Has this been added? Is it available in 2012? If so, we're unable to find it.

[CelticDesignServices]

Here's what I need to dimension to:

[Curtis_Waguespack]

Hi CelticDesignServices, 

First, let me be so bold as to question whether that hole would really be angled in what appears to be a sheet metal part. My thought being that it would be placed in the flat and would not be at that angle. 

But assuming that it is drilled at an angle, try this:

• In the model create a Work Point using the right-click Loop Select method.
• Then return to the drawing view and expand the view node in the browser and locate the work point.
• Then right-click on the work point node and choose Include, this will place a centermark.
• Now place your dimension using the centermark
• Then right-click the centermark and choose Visibility to hide it, leaving just your centerline.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[CelticDesignServices]

Thanks Curtis.

Actually the pic I supplied is not an actual part, I was just playing around with the Sheet Metal Bend tables and had that "dummy" part open at the time this question came up from a co-worker. Thus is quickly extruded a hole at an angle to demonstrate the inability to dimension to the intersection of an edge and a CL.

Sorry for the confusion.

As far as your work-around, it should work, but dang.....why can't Inventor do something like this in the dimension command, it seems fairly simple and obvious.

Hello? AutoDesk? Are you listening?

[Curtis_Waguespack]

Hi CelticDesignServices,

It dawned on me after I posted earlier that we can just use the centerline end point to place the dimension and then drag and drop the dimension snap to the intersection point after the dimension is placed, as well. Although to do so you have to "scrub over" the lines in a particular order to get it to snap to the correct place.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Edit:

I just noticed you've already commented on that solution in another thread:

http://forums.autodesk.com/t5/Autodesk-Inventor/Oridanate-dimension-problem/td-p/597031