I have a skeletal master part and in one of the sketches one of the dimensions flips direction, if this dimension was defined with a positive direction of 12 o'clock(20120725-DimensionChangeDirection0.jpg), over time and changes, the
positive direction will flip to now being 6 o'clock(20120725-DimensionChangeDirection1.jpg) and it doesn't break the model, but I now have less holes than required.
Anyone else seen this? If so, any recommendations?
I will not upload models.
Solved! Go to Solution.
Many times ... one of the problems with both linear and angular dimensions within a sketch is that they don't actually have an associated vector direction or rotational reference.
Depending on the complexity of the sketch/part; one solution is to use workplanes (which do have direction vectors) and project them into the sketch to define your geometry.
The only time I have seen this happen is if at some point the value of the dimension was set to 0, then changed to a non-zero value.
As conklinjm says, the sketch dimensions don't have an absolute direction. So when changing a zero value to a non-zero value, the direction that it decides to go is unpredictable.
If you know that your parameters can have values such that your dimension can be 0, then it is best to define that dimension in another way to avoid this problem.
Your solution of Workplanes is superb conklin, thank you. :-)
I figured there may be a problem with direction when a dimension value = 0, but when I analysed the values these are occurrences of zero are very few, however pretty much every time I edited this assembly, the holes are flipping direction.
Thanks for you help people.
I am having this exact problem. Would you provide an example or more detail of projecting the workplane into the sketch to resovle the problem?
Under my circumstances, I had a dimension that was controlling the position of a hole on a 2D sketch, an equation was driving the dimension. In order to have a Workplane drive the position, I copied the quation from the dimension and changed it to a driven dimension type, the sketch was closed, EOP marker was moved above the sketch and a workplane was then created using the equation from the dimension, I endured a couple of circular reference errors with the equation but managed to remove them by changing the equation properties. I moved the EOP marker back to the bottom, edited the sketch to now include the newly created workplane and constrained my hole centre to the projected geometry.
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