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Jun 18, 2016 1:44 AM UTC
Question

Existing bug in Creo Parametric 4 sketching

I apologize if I am not supposed to post existing bugs but there is one issue in sketching that I really would like to see resolved and it seems that it should be fixable.

When you have slanted lines or splines connecting each other and place a radii it causes movement in the 2 entities once the radii has been modified.

The only way this can be resolved is to replace the dimensions that once held the sketch together.

Below is a slanted rectangle; notice that there are locked dimension for horizontal vertical and angular.

slide 1.JPG

When you apply a radii it removes the locked horizontal and vertical dimensions and replaces this with an unwanted radii center horizontal and vertical dimension.

slide 2.JPG

As soon as you modify the radii it moves the position of the slanted rectangle.  See how the horizontal and vertical locked dimensions no longer match.

slide 3.JPG

I would really like to see this fixed.  For every single radii on slanted lines or splines you have to replace the locked dimensions to the construction entity intersection.

    4 replies

    Jun 20, 2016 3:22 PM UTC

    This isn't a bug, per se. Perhaps the behavior isn't what you're looking for, but it does follow a predictable behavior.

    What seems to be happening here is that if you have dimensions to the vertex of the rectangle (even if they are locked) they get removed when a fillet is placed on that corner. This has a logical basis because technically that vertex is no longer in the geometry and so the dimension cannot be preserved. The sketcher does create a construction vertex in place of where the old geometry vertex was, but this isn't the same ID as the vertex that was there previously. The solver then attempts to create some new dimensions in order to keep the sketch fully constrained and it chooses to use the center of the radius as the point to be dimensioned. Once these dimensions are in place, the sketcher will preserve these dimensions during subsequent modifications of the radius value. So, the center of the radius remains fixed and the arc will get larger or smaller and thus move the rest of the sketch due to the tangency constraints.

    It sounds like what you would like is for the sketcher to create new dimensions to the construction vertex that gets added when the fillet is applied instead of creating dimensions to the center of the arc. This seems to be a matter or preference, because I can imagine situations where the user wants and expects the dimension to go to the arc center instead of the construction vertex. We can look into making some more intelligent assumptions to the effect that if a dimension exists to the vertex that is removed by a fillet, then the software should replace it with a new dimension to the construction vertex instead of to the arc center. This behavior change would not be a bug fix, however, since there doesn't appear to be a bug here anyway.

    The other thing you can do as a workaround, is to create a point at the vertex of the rectangle and then dimension to this point instead of to the vertex. Then, when you create a fillet on the corner, the dimensions will stay attached to the point and not be removed. Subsequent changes to the radius of the fillet will not "move" the sketch since its location remains fixed according to the point.

    I hope this helps.

    -Raphael

    pimmAuthor
    Jun 20, 2016 9:02 PM UTC

    This seems to be a matter or preference, because I can imagine situations where the user wants and expects the dimension to go to the arc center instead of the construction vertex.

    This really is not a matter of preference.  I have placed "locked" horizontal and vertical dimensions to the sharp corner of intersection.  It should be harder for me to remove my own locked dimensions than it would be for the shape to distort because it was automatically removed.  If anything it would be nice if there was a prompt towards removing locked dimensions when the original sketch corner is pared away just in case it was intentional.

    The radii application does work correctly when rectangles are perfectly horizontal and vertical.

    If I were to place the locked dimensions  to the radii center then the rectangular sides should move with the change.

    We can look into making some more intelligent assumptions to the effect that if a dimension exists to the vertex that is removed by a fillet, then the software should replace it with a new dimension to the construction vertex instead of to the arc center.

    The software does have the intelligence to replace the old corner with construction entities.  If it could only go one step further and remember the locked dimension that was removed.

    I will look at what you say in regards to placing a point on the intersection of the lock dimensions.

    I appreciate you looking at this.  I am hoping that this is a resolvable issue.

    Jun 20, 2016 10:33 PM UTC

    This really is not a matter of preference.  I have placed "locked" horizontal and vertical dimensions to the sharp corner of intersection.  It should be harder for me to remove my own locked dimensions than it would be for the shape to distort because it was automatically removed.  If anything it would be nice if there was a prompt towards removing locked dimensions when the original sketch corner is pared away just in case it was intentional.

    "Locked" dimension only means that the value of the dimension will be preserved during modification of the sketch - particularly when dragging portions of the sketch. It does not currently mean that the dimension cannot be removed from the sketch if the entity to which it is attached is deleted. In this case, the vertex to which the dimension is attached is being removed from the sketch by the fillet, so it follows that the dimension should go away.

    I agree that there is room for improvement here in that we could try to detect a strong or a locked dimension to the vertex and if one is found we could create a new dimension in its place that would now refer to the construction entity vertex left behind by the fillet. This would give the appearance of preserving the original dimension and also would better preserve the design intent.

    I'll check with development and see what they say about it. I don't hold out much hope that this could still be done in Creo 4.0, however, since we're focused on getting the bugs fixed for F000 later this year.