During making idw's encountered the following problem.
We have an exact measure of 20. When placing the dimension in the idw this becomes 19.9993... . How is that possible?
A dimension is an exact value and I expect the drawing to represent that in an accurate way.
In a few drawings this error even becoms to 3/100 afwijking on a dimension.
We make models/drawings in hundreds of millimeters.
We count on the fact that the measure in the drawing is the exact representation of the model.
Is this a more common problem. I know that these are double curved surfaces but a top view is a top view. in my opinion.
This is the first time I encountered this problem.
How can we solve this?
Solved! Go to Solution.
Solved by JDMather. Go to Solution.
When I dimension a cross section at a depth to get a full circle the dimension is right.
Right view is not actually a circle because the extrusion goes thru a circle
Dear Erik
I recreated your issue from the dimensions in the pdf. Your part is fine, the issue is the centre points.
The centre points are the centres of the part geometry not the projected circles that you are expecting.
Hopefully someone cleverer than I can tell you how to fix this.
Sorry I can't be of more help.
Mark
HI!
The question is... youre not measuring the top view... you are measuring the projection of the sketch in a curved surface.
If you want the real 2D dimensions, create a new sketch, project the line between the circles.
In drawing, "Get Model Sketches" and dimension the line... you will have the true 2D values.
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What if you use the same dimensions you used to create the geometry?
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As stated previously, what you are seeing is a function of the projected geometry.
Instead of manually dimensioning the part, why not simply RETRIEVE the model dimensions that were used to create the model.
All given solutions are correct and usable.
But a top view is a topview.
And if the measure on drawing is a result of he sketch but not given "hard" in the sketch.
We have drawings where the dimension on a radius of 7.25 varies between 7.23 and 7.27 in a round off this can give 1/10 of milimeters.
I was of the oppinion that all measures on a drawing are "correct".
That I did not have to check them again on how accurate they are. But now I have to check every dimension. That should not be ....
@Anonymous wrote:
But a top view is a topview.
You are thinking like you drew it in 2D cad and in that case yes a top view is a top view.
But Inventor gives you geometry that is the same as the 3D model. What you are clicking on to create the dimension of 19.99??? is not a circle, it is a "polyline".
Sometimes having the 2D view being that accurate is great, other times not so much. Grin
I have a similar problem but it's not from part to drawing; it's totally within the part itself.
I have a part with two holes. I put a work axis in each hole, create a work plane thru the two work axes, and then created a workplane 6mm from the first workplane.
Then I create a surface on the second workplane. It should be 6mm from the axes of the holes but when I measure the distance, I get a number like 5.99999999847020. Certainly not a big error but enough to break assembly constraints.
This is just one example of many instances of similar happenings. I know there is no issue of holes not perpendicular to surface or things like that.
Hi! I believe it is actually a bug in the measure tool. Such imprecision should not occur in analytical geometry (plane, cylinder, cone, sphere, and torus). Please share an example that exhibits the behavior. I will work with the project team to understand the imprecision better.
Many thanks!
Just tried to duplicate the same geometry and this time it measures appropriately. But I know I wasn't seeing things; repeatedly measured and got the same [incorrect] results.