Strange discrepancy between model and drawing dimensions.

[erikjan.koeze]

While trying to figure out why I can not get precise dimensions on a specific part, I chose to remodel it to make sure nothing I did was wrong. Results are the same...

How do I get the dimension to accurately display as 20mm without rounding it to a lesser precision?

See attachments for screenshots of model and drawing of the same section.

[CCarreiras]

There's no attachements... anyway, i believe this should help you:

https://knowledge.autodesk.com/search-result/caas/simplecontent/content/inventor-places-incorrect-di...

[erikjan.koeze]

Thanks. Screenshots are attached now.

[CCarreiras]

Well.... we can do nothing with images, we have to check the model....

[erikjan.koeze]

I have attached the files (idw and ipt). 

Running Inventor 2022.3 build 350

[CCarreiras]

I guess the template has some issue, try another template.

For me, it works well...

[erikjan.koeze]

Can you try with a higher precision? Dimension is 20.00015 in my drawing.

[CCarreiras]

If I set bigger precision, I will have the same result as you.

I guess this is due to the curved surface of the tube.

...but, the question is... why do you need to increase precision to that level?!

[erikjan.koeze]

I don't need the precision. I'm curious what would cause this. Is it my modelling or is it something strange. 

If I place the same dimension in another view, again on the centerline, the dimension IS correct, which makes it even more peculiar...

[CCarreiras]

The dimensions are placed based on the geometry projection.

I think this issue occurs due to the projected hole geometry in the curved tube surface, which adds some imprecision... ...but is a "residual imprecision", regarding product documentation and the precision required for that, is more than enough, don't worry about that.

[johnsonshiue]

Hi Erikjan,

This is an Inventor limitation. The reason why the diameter dimensions are slightly off is because the edges associated with the dimensions are intersection curves (between two perpendicular cylinders). The geometry is spline. As a result, the project of the spline edge is also a spline. Inventor utilizes approximation to get the diameter value within a predefined tolerance.

If the precision is set to 0.001, this behavior will not be seen. This is why Carlos thinks a different template file matters (precision settings).

We have been investigating a solution. But, there is no good solution yet. It is because the circular approximation is leveraged in many places. To get a true reading, the tolerance needs to be very high or there needs to be a special rule only applicable to the intersection between perpendicular cylinders.

Many thanks!