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Dimensions flipping direction - IV2013

13 REPLIES 13
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Message 1 of 14
Scott_Stubbington
7497 Views, 13 Replies

Dimensions flipping direction - IV2013

Hello,

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.

 

Thanks

 

Scott

13 REPLIES 13
Message 2 of 14

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.

 

HTH

Message 3 of 14

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.

Message 4 of 14

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.

 

Regards

 

Scott

Message 5 of 14

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? 

Message 6 of 14

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.

 

HTH

 

Scott

Message 7 of 14

Is there a better solution to this problem now, a few years later? If a dimension can possibly have the value of 0 which would cause it to break, is it better to supress and unsupress dependencies? I have a complex master part where integrating all those workplanes would be a very tedious project. 

Message 8 of 14
torbjorn
in reply to: tobias.fischer

As far as I know nothing is changed (but I am still on 2017).

 

Actually the solver seems to know the direction of the dimension, but it looks like Autodesk have placed some code on top of this ro remove direction.

 

You can see this if you place a dimension between a fully constrained line an an unconstrained. Change a dimension to driven and pull the dimensioned line to opposite side of the fixed line. Then it gets negative. If you change it back to driving it will change sign without moving the line. I think it shows that a dimension actually has a direction vector, but for some reason we are not allowed to use it.

 

Torbjørn

Message 9 of 14
guilloryt
in reply to: tobias.fischer

The solution we generally use is to create dimensions by referencing geometry such that to get the results require the value never goes to zero.

 

In our apps we are generating models from a master model by driving it parametricallly from a tables the user defines. Our issue was how to allow the user to enter a value of zero when the model being generated required it.

 

The solution we generally use is to set the dimension that is driving the geometry such that the value never goes to zero ( ex.. set the base reference of the dimension to the part od or id). Then create a user parameter to allow the user to enter a value of zero. And use that user parameter value in a formula in the parameter for the dimension that is driving the geometry.

 

In our drawings dimension we always pull reference parameters from the model. For these we create a referenced dimension that can go to zero and not cause any issues.

Message 10 of 14
tobias.fischer
in reply to: guilloryt

Things like These happened to me in ilogic (example). Inventor randomly changed the value of the angle into something else, even tho the line Colors told me they were fully certain. i take the values from a list, they arent even 0 often, but it switches directions. Maybe it has to do with the order in which the dimensions are updated or something. i use values for my dimensions that i get from linked Excel Parameters (this Image is just an example of what happens to me, here the Parameters are not linked).

 

 direction change.PNG

any suggestions what im doing wrong? is working with angles problematic?

Message 11 of 14
guilloryt
in reply to: tobias.fischer

Hard for me to be certain by only looking at that sketch. But guessing it is related to the fact that dimensions don't have a direction component (which is the reason for the suggestion about workplanes).

 

But can tell you that our problems are very difficult to reproduce and isolate. A good example that would often occur is with the width of a groove. If you dimension it such to allow the user to enter a 0 width value.. the sketch defining the two groove walls collapse on it self. The real issue i think comes if you try to take the vers of the model you just have updated.. that is having a 0 groove width and then update it with a value. Usually it will work... but sometimes not. What it appears to me is the dimension really does not have a direction component... so sometimes depending on the order Inventor resolves parameter updates.. the sketch will invert and the sketch line for the right side groove wall will switch to the left side. (offhand that looks similar to your angle issue(

 

One item I failed to mention about our process is that when generating models from a master.. if you always start with a master that has values >0  for all parameters that are drving geometry there won't be an issue. You can always collapse the sketch geometry.. but any time you update a dimension value  that is already zero will often produce unpredictable results.

 

Not sure what you are doing.. but if you are generating sets of member models from a master design it might be the best option ..to open a fresh copy of the master (that does not have any dimens with 0 values) before creating a new member.

Message 12 of 14
tobias.fischer
in reply to: guilloryt

The tip with Always opening a template master file where all values are more than 0 is a good idea.

In my opinion autodesk should simply implement a directional constraint. Or does something like this already exist? 

 

Message 13 of 14

We need to dimension the sketch a bit differently.

For example: a rectangular bar with a series of holes.

We usually draw the rect and dimension first hole to one end of the rect and pattern the holes.

If we shorten the rect, the first hole will move outside the rect.

 

Instead, we can dimension the first hole to the center of the rect with equation.  This will prevent the hole from moving outside.  Unless the rect length was changed too short.

 

On the angle changing, try dimension to the center of the rad to prevent it from moving higher.

 

The problem is the sequence of solving all the dimensions and geometries in the software.

Message 14 of 14

Hi! I have seen this behavior before. This has something to do with the geometry, where dimensions are placed, and how much the change in dimension is applied. Sometimes, the behavior can seem random. If you have a case consistently reproduce the behavior, please share it here. I will follow up with the project team to see what we can do.

Many thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer

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