2d sketches constrained to the provided plane?

[katopodis_odys]

Hi guys, I noticed some strange behavior with circles drawn on a plane (I didn't create an offset plane, I used 3d geometry as the pane, which wasn't touched throughout my edits.

My goal was to create tubes and route them.

The circles are a 2d sketch on a plane (used as marks where the cross-section of the tubes will be positioned) and I use a 3d sketch for the path for the tube command. 

When a change in the parameters (distance between center was made universally) was made, circles (on this specific Sketch) were "bend" outside the 2d plane in order to satisfy the change).

I was under the impression that the sketch was constrained on the provided when designing 2d plane.

Is this not the case with fusion ?

I read in a post that this maybe would have been the case if I had constructed an offset plane (same plane as before but constructed one). 

Can anyone explain?

[g-andresen]

Hi,

please describe what you want to achieve in the end, add a picture of such an object and share the file

File > export > save as f3d on local drive  > attach to post.

günther

[katopodis_odys]

Hi @g-andresen. I solved my problem the hard way (re drawing). It is a theoretical question aiming to increase my understanding of sketching best practices.  The goal is in future designs to only change my defined parameters and the tubing to play along nicely. I can't share the file, but I could create an "equivalent" case (busy on the job, will have to wait).

Thanks for the quick response. 😁

[laughingcreek]

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@katopodis_odys wrote:...I was under the impression that the sketch was constrained on the provided when designing 2d plane.

Is this not the case with fusion ?...

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nope.  once a 2d sketch becomes a 3d sketches you have to add more constraints to keep circles on their plane.

[jeff_strater · Accepted solution]

"I was under the impression that the sketch was constrained on the provided when designing 2d plane.

Is this not the case with fusion ?"

The real answer is "yes and no".  All sketches in Fusion are the same.  There is no "2D sketch" or "3D sketch".  All sketches can contain geometry that is on the sketch plane or not on the sketch plane.  For instance, if you sketch a circle on the sketch plane, you can use the Move command to drag that circle away from the plane, or rotate it.  So, inherently, all Fusion sketch geometry is 3D.  There is no constraint that will glue a geometry to the plane.

Now, if a sketch contains only 2D geometry and constraints, I am not aware of a case that would pull a sketch plane geometry away from the plane.  If the sketch contains non-planar geometry with constraints to the planar geometry, yes, I suppose that can happen.  If you have a case where purely 2D geometry is being moved away from the plane, I'd be interested in seeing that, as I would consider that a bug.

[katopodis_odys]

Hi, @jeff_strater thanks for elaborating on the matter.

"Now, if a sketch contains only 2D geometry and constraints, I am not aware of a case that would pull a sketch plane geometry away from the plane.  If the sketch contains non-planar geometry with constraints to the planar geometry, yes, I suppose that can happen.  If you have a case where purely 2D geometry is being moved away from the plane, I'd be interested in seeing that, as I would consider that a bug." 

I checked again, and it seems that the sketch includes non-planar geometry by accident.

Sharing the complete file is not an option, but I could copy the "2d" sketch (and the 3d sketch that uses it) to an empty file, if you like. (though I think a lot of information will be lost that way).