topic Re: Drawing - Ordinate dimension from centre line to centre of feature in Inventor Forum

Drawing - Ordinate dimension from centre line to centre of feature

SEC_MECH — Wed, 15 Jun 2022 03:58:08 GMT

Hi,

I want to use ordinate dimensions using the centre line as my origin.

I want to dimension to the centre of a feature.

The ordinate dimension tool does not allow me to select the centre line as the origin. I must select an edge.

The ordinate dimension tool does not allow me to select the centre of my feature. I must select an edge.

How can I use ordinate dimensions from a centre line to the centre of a feature.

I want the ordinate dimension equivalent of this:

Re: Drawing - Ordinate dimension from centre line to centre of feature

daniem — Wed, 15 Jun 2022 05:07:09 GMT

I usually used an edge, so I cant comment on previous versions.

As for inventor 2023, I can place the origin on the middle of the edge. If the part origin is in the center of the part you can rmb and "include" it in you drawing and use that is the origin.

After placing the dims you can move them to where ever you want aka the center point of the cut out.

This is a workaround and might be double work, but it is the only way I know for this.

Maybe suggest it as a feature.

Re: Drawing - Ordinate dimension from centre line to centre of feature

SEC_MECH — Wed, 15 Jun 2022 05:40:34 GMT

Thanks @daniem.

That worked after a fashion.

Re: Drawing - Ordinate dimension from centre line to centre of feature

SBix26 — Wed, 15 Jun 2022 18:52:43 GMT

First, unselect Application Options > Drawing > Enable ordinate dimension geometry selection:

Then use the Ordinate Dimension Set tool to create your dimensions. This tool allows you to choose a centerline as origin, because it is selecting only a single direction. [The view origin required by the Ordinate Dimension tool sets the origin for both directions; centerline ends are not reliable for one of those directions. However, it ought to allow the selection of an intersection between centerlines!]

In any case, this is what I could produce with the option set as above and using the Ordinate Dimension Set tool:

The best workaround for this is to simply make sure that your model is created symmetrically around the origin, then include the origin point in your drawing view. This point is selectable for the view origin.

Actually, I don't think this should be considered a workaround for this case-- this would be a better practice than using bisector lines to define the view origin.

Sam B

Inventor Pro 2023.0.1 | Windows 10 Home 21H2

Re: Drawing - Ordinate dimension from centre line to centre of feature

SEC_MECH — Wed, 15 Jun 2022 22:44:12 GMT

Thanks @SBix26 . I already had that checked. The Ordinate set does allow me to choose the centre line.

@daniem opened my eyes when he said that I had to place the point on the geometry, nearest to the centre of the feature that I actually want to dimension, and then move it once the ordinate dimension was established. I have products with 150 square holes in a single plate so I have to place 300 ordinate dimensions (150 in X and 150 in Y) and then tweak every single one. Not intuitive and not helpful. Autodesk should improve this.

Re: Drawing - Ordinate dimension from centre line to centre of feature

SBix26 — Thu, 16 Jun 2022 00:40:49 GMT

@SEC_MECH wrote:

Thanks @SBix26 . I already had that checked.

The answer is to uncheck it. Then you can select center points of lines, as I showed in the image I included. I didn't move any of those dimensions after placement, that's where I placed them to begin with. But this is only possible if you uncheck "Enable ordinate dimension geometry selection".

Sam B

Inventor Pro 2023.0.1 | Windows 10 Home 21H2