How do I dimension project cut edges?

[Derek00111]

When using Project Cut Edges command, and the cut geometry is projected onto a work plane, how do you then use those edges to produce general dimensions, since the projection is completely constrained automatically? I am trying to preserve the idea that it is a projection and not delete the constraints.

I attached a page from the tutorial I am trying to follow. I cannot understand how the dimension is produced without it being a driven dimension.

[JDMather]

Attach your *.ipt file here.

The Projected geometry itself does not need to be dimensioned, only any new geometry added to the sketch.

[Derek00111]

part file has been attached.

[SBix26]

The two dimensions shown in the tutorial are defining the circle that is added to the sketch, not the projected geometry.  After placing the circle, the location of the circle center and the circle diameter are undefined, requiring three dimensions to completely define (the message at the right end of the status bar says "3 dimensions needed").

One of the location dimensions is taken care of by constraining the center to the projected line; the other with the .060 dimension.  The last degree of freedom in the sketch is the circle diameter, and the applied .125 dimension resolves that.

Note that you can turn on a display of remaining degrees of freedom while editing a sketch:

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Sam B

Inventor Pro 2023.1 | Windows 10 Home 21H2

[JDMather]

@Derek00111 

Your Sketch2 is not fully defined - it should be placed at the Origin Center Point.

Was this not covered in the tutorial instructions?

Work Plane 1 and Axis are not needed if original sketch had been placed at the Origin.

Sketch6 location is not defined in space - it should be centered at Origin.

Sketch9 is missing diameter dimension of the circle. 

Did the instructions not cover these steps?

I do not see a sketch with Projected Cut Edges in the file that you Attached?

On Step 4 I had trouble picking the left line for .06 dimension looking straight at the model.

If I rotated it a bit it was easier to pick the line (or endpoint).

See Attached file for how I place my sketches at the Origin....

Also, when selecting the line to place the small circle be careful to NOT select the midpoint of the line as the midpoint is very close the the intended location of the circle.

Always, always, always (at least as a beginner) model with symmetry about the Origin Center Point.

This is the foundation of the BORN Technique of modeling.

[Derek00111]

The file I attached is the file they provided to begin with. The origin point was their decision. The tutorial moves on from there.

First two pages before the page I attached require work axis to be centered at the taper, which goes through the origin you want. XZ plane is rotated to 0 going through the origin you speak of. Not posting the entire 10 page exercise, not sure if that's allowed.

Sketch9 diameter not in exercise.

Dimension is based off the point, not the project cut edge. I see now. 

[JDMather]

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@Derek00111 wrote:

The file I attached is the file they provided to begin with. The origin point was their decision. The tutorial moves on from there.

First two pages before the page I attached require work axis to be centered at the taper…

Sketch9 diameter not in exercise.

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@Derek00111 
I hope their intention was to have you learn how to create Axis and Workplane and that somewhere in the learning materials they demonstrate more robust modeling techniques.

If not, I would be concerned about the quality of the training material.

[johnsonshiue]

Hi! Just by reading the pdf tutorial, it seems that the process is reversed. There isn't anything wrong with using Project Cut Edge here. But, it does feel odd to me. The dimensions that need to be documented in the drawing should mostly be driving dimensions in the sketches or features.

The particular modeling approach described in the tutorial seems to separate modeling from documentation. It means somebody creates the model and somebody else creates the drawing. We do have some customers using the same approach. There isn't anything wrong wit that. It works well for imported parts or when the modeling is mostly done.

Many thanks!