(BUG) Drawing dimensions do not match model

[Anonymous]

I am creating a drawing for a part, but for some reason certain dimensions to not match the model. What is weird is when I click on the parts I want to measure, it has the correct measurement. Then, once I click to place the measurement down it changes. 

Picture 1 is before placing the dimension, picture 2 is after, and picture 3 is the part.

[mcgyvr]

Can you post your idw file and ipt file? They are usually much more helpful in determining the issue vs images..

[Anonymous]

Try changing your leading zeros on your drawing or your sketch dims.

It is rounding the digits for you automatically. The sketch is rounding to three digits while the drawing is not rounding the trailing .3127 to .313

also to note that if the 5th number is large such as .31298 it could round it to three digits even if four is chosen.

here's a simple sketch showing the dim difference/roundinghere's how to set the dim rounding on the drawing.

[Anonymous]

The part that I was looking at there is named "Jack two holes"

[Anonymous]

That's my mistake, in the model it is 0.3125 inches.

The thing that's really confusing is the dimension matches until I confirm placing it on the drawing (original pictures 1 and 2).

[Anonymous]

First I would check the constraints for the dim's on the model sketch first. make sure your on the object sketch projected geometry not on the extruded face/space that may be out slightly.

next i would see if the center position of the holes are the same on the drawing or did it change the dimension and auto constrain to a space around the object. Check to see if any of your pages have sketches on it.

[Anonymous]

The model sketch is on the origin plane

There are no other sketches on the drawing

I think you're missing the point of the issue, when I choose what to measure it shows the correct number, but for some reason once I place the measurement it changes. One of my co-workers is running into the same issue, though I don't know his exact circumstances.

[Anonymous]

I don't mean to cause distress however this is more specifically what I mean.

The projected point may be out from the model to the sketch.

as the sketch will use the geometric line around the arc of the circle as opposed to the point that is created in the sketch. i would just confirm that the point on the sketch is attached properly to the projected dim. i will take a closer look at the models them selves later tonight though as these are hand drawn.

[Anonymous]

I believe I understand it, and as far as I can tell the point is correctly positioned on the arc.

Something else odd that I just tried is creating a section view from the same angle. This time the dimension is correct.

[Frederick_Law]

I think something is wrong:

[Anonymous]

I'm curious does it reset if you command the front of the view cube to the appropriate plane?choose sketch planechoose view tab. choose faceright click cube and set view or reset frontreset cube

[Frederick_Law]

I start with a new part using my templates and got same problem.

[Anonymous]

That doesn't change anything for me, I still run into the same issue. I don't understand how that would change anything unless it was misaligned initially.

[Frederick_Law]

I've reported and AutoDESK confirmed its a bug.

They're investigating.

[Anonymous]

I'm not sure its a bug though. After confirming with a colleague over the matter he suggested the same issue that I was saying. That when you refer the dimension of a spherical object that it can dimension to any point rather than center of object. although the picture is showing a front 2D object the 3D image still exists within the drawings back ground. So instead of it grabbing the exact center of the sphere it is grabbing another random point that is very close. 

He also said that for these type of drawings absolute best practice is to use the center of object on the drawing for a center line to have a better and more accurate drawing. As opposed to using the extra view or section drawing to get the center line.

[Anonymous]

If it's dimensioning to a random point instead of the center of the object that sounds like a bug to me.

I set up the section view more as an example. But I did it because I could not find any way to get the correct dimension on the other view.

[Frederick_Law]

IV use a tangent point on the radius.  I've dimension other parts before and it worked.

Same as dimensioning to the top and bottom radius of the rod.  It works perfectly there.  No reason it doesn't work on the cut.  Even my dimension from center mark to center mark are wrong.

I found the problem in the file.

Then I start new and redraw everything, still got the problem.

So its not mis-alignment or file corruption.

AD verified it happen in multiple versions of IV.  Including 'future' version.

Retrieved dimensions does work.  So it could be a workaround for now.

[johnsonshiue]

Hi Guys,

This is a limitation in Inventor at the moment. The reason why there is slight discrepancy in dimension is due to the spline approximation. The edges of interest are created by cylindrical cut. The faces are cylinder. However, the edges are intersecting spline edges. When such edges are projected to the view plane, they are approximated to the closest arc. This approximation can lead to dimensional difference.

Just like experts mentioned here, you may want to retrieve model dimensions or include the model sketches in the drawing.

We are aware of the deficiency. We are working on a solution for future releases.

Many thanks!

[Yijiang.Cai]

@Anonymous , this issue has been tracked in our system, and the development team are investigating it. Based on the investigation, the key reason is related to the face created by cut, it is actually a nurb curve face instead of a cylinder. So in drawing the circle is the approximation instead. This causes the difference of that circle radius.

[Anonymous]

Thanks for the info. Now that I know how it happens it should be easier to handle when it comes up again until it's fixed.

@Yijiang.Cai That makes sense why the dimensions are off. But do you know why the correct dimension is shown prior to confirming the dimension's position? It seems like it knows what the correct value is, but then changes to the incorrect approximation.