Drawing ordinate dimensions on turned parts best practices?

[HelmholtzW]

Attached is sample part and drawing. I'm finding it impossible to create ordinate dimensions from the centerline for turned parts. Even though the centerline is point 0, the ordinate dimension tool gives seemingly arbitrary numbers in that axis. 

What am I missing here? The spline feature cannot be dimensioned in any way at all so this is another issue. I can't seem to add any points that can then be dimensioned.

In order for this part to go to production the drawing must be fully dimensioned. All points of the spline must be marked in both X and Z axis. All arc center points as well. 

Would love to see some examples of properly drawn parts for turning. Thanks!

[g-andresen]

Hi,

There's a workaround.
If you activate the sketch in the browser in drawing mode you will get spline points for dimensioning. Diameters can only be dimensioned if the spline has been mirrored in sketch mode. Otherwise only radius is possible.

regards

günther

[HughesTooling]

If you draw points on the spline then set the sketch to visible in the 2d workspace the points show. The spline points will not show so just smap another ordinary point on top of them in the model sketch.

Mark

[HughesTooling]

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@g-andresen wrote:

Hi,

There's a workaround.
If you activate the sketch in the browser in drawing mode you will get spline points for dimensioning.

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@g-andresen  I don't get the spline points unless I draw an ordinary point on top of them. Are you using a Fit Point or Control Point spline?

Mark

Mark

[HughesTooling]

@HelmholtzW  Here's your part after mirroring the spline then snapping points to each spline point. File's attached.

Mark

[g-andresen]

Hi Mark,

It works with both (fit point and control point).

The green crosses are no control points but characteristic points of the spline.

regards

günther

[HughesTooling]

Yes I noticed those but they're not necessary in a useful place, nor are the actual spline points. I guess you might be better off just adding points at places you can measure.

Mark

[HelmholtzW]

So that's actually good workaround but there are caveats. Thanks for posting the revised file for me.

After your part is modeled create a new final sketch and project the part into the sketch. This new sketch should be the final item in your timeline. Add any points that you want to dimension on your drawing into this sketch. This way you capture any changes you made to your model like fillets, chamfers, etc after you did your revolve. Don't use your original part sketch in your drawing or you will loose any changes you made after you completed that sketch in the timeline!

Mirrored points don't seem to show up in the drawing workspace. You need to add a point over top of a mirrored point in your sketch. Mirroring the sketch is only necessary if you require dimensions in diameter. 

Make note of your sketch orientation. If sketch is visible as 'TOP' in modeling you need to make sure part is oriented to 'TOP' in the drawing or your sketch won't be visible. 

Certainly not intuitive but this produces the necessary result and the drawing should update correctly if any changes are made to the model.

[HughesTooling · Accepted solution]

@HelmholtzW  I been thinking about this some more and like you figured a second sketch is a better way to go. In the attached I created a Project - Intersect from the surface created from the spline, then added construction lines and dimensioned their position so they are in useful places. Still needed to add points at the end of each line (stacked points) before they show in the drawing.

Sketch in model workspace

And drawing

File's attached.

Mark

[HelmholtzW]

I put your method to the real world test and it works great. I was able to create a properly dimensioned drawing, of a real part, much quicker and more reliably then before.

By creating the sketch before you create your drawing you can put points in more meaningful locations whether it is defining a spline, or the center point of arcs. 

thanks for posting the example files.