Sketch weird behaviour (2D to 3D?)

[Anonymous]

Hi,

I am quite new to Fusion 360.

I as struggling with a strange behavior of one of my sketches. Some of the dimensions in the sketch are not displayed properly. I am not able to add new dimensions, etc. The last thing I noticed is that if I position the POV from the side it looks like the sketch has thickness to it or that it is not on one plane but rather is a 3D sketch. I have no idea of how that happened since I selected a sketch plane to begin with.

How can I see if a given sketch is 2D or 3D?

How can I convert for one to the other?

What caused my sketch to become 3D?

Why am I not able to add any dimensions to the current sketch?

Many questions but I think they are all related.

I appreciate your input.

[Anonymous]

Just a small update. I checked and verified that the 3D sketching option is disabled in my preferences (see attached).

[TheCADWhisperer]

File>Export and then Attach your *.f3d file here.

For beginners (and even experienced)  recommend that they start over frequently till they discover what actions result in unexpected behaviors.  I often learn more from when things go wrong than when the go right from the start.

[jeff_strater · Accepted solution]

if you have used the Move command while in sketch, you may have dragged in the sketch Z direction.  To see if any geometry is not 2D, select it and right click.  If the geometry is not on the sketch plane, you will see "Move to sketch plane" in the context menu.  This command can be used to also force geometry onto the sketch plane, if it inadvertently has gotten moved.

[hpekristiansen]

How can I see if a given sketch is 2D or 3D?

All sketches are 3D.

How can I convert for one to the other?

You can not. -All sketches are 3D.

What caused my sketch to become 3D?

All sketches are 3D.

With the 3D enabled in your sketch or preferences,

you can accidentally snap to a point outside of your sketch plane.

Why am I not able to add any dimensions to the current sketch?

You can not add a 3D dimension. (but you should be able to add normal dimensions in the sketch plane.)

If you read this, all will make more sense:

https://www.autodesk.com/products/fusion-360/blog/fusion-360-tech-tip-sketching/

[laughingcreek]

@hpekristiansen -Continuously saying all sketches are 3d is miss-leading and confusing.  Yes, all sketch entities exist in a 3d model, and are therefore technically  "3d".  But within the context of how fusion works, there is a difference between a sketch that has all elements on a single plane (i.e. a 2D sketch) and one that has elements that exist off the sketch plane (a 3D sketch).  Within the context of fusion, if all elements of a sketch are entirely on the defined sketch plane, it is considered to be a 2D sketch. 

@jeff_strater -I've suggested in the past having some kind of indicator (maybe a "3D" icon on the sketch in the browser, next to the lock symbol for fully defined?) to indicate when a sketch has "gone 3d", either by intent or accident.  Is there any discussion of adding this over at AD?  Having to do a manual check on individual elements is not a great way to find accidental 3d objects, and doesn't work at all when it's a 3d projection.

[hpekristiansen]

I do not agree.

All sketches are 3D in Fusion, in the sense that they can contain points in 3D. Sure if all the points happens to be in one plane(the sketch plane), then the we can considered it to be 2D.

What confuses OP, and a lot of other people is that they believe that there is a difference, and that you can convert or set the dimensions of a sketch. This confusion is furthered by the not very well explained check box "3D sketch" in sketch mode.

I was the only one answering OP's questions(as best as I could).

"within the context of how fusion works, there is a difference..." - really!!? Please explain this - maybe I am wrong.

[davebYYPCU]

I think you have conceded yourself, the difference is planar against non planar, 

far more functionality available with planar sketches.

[hpekristiansen]

Please do name one functionality that is not available for a sketch with a point outside of the sketch plane.

I am not trying to spread doubt or misinformation - I am genuinely interested.

[davebYYPCU]

All Dimensions, profiles, Some constraints are not available in non planar sketches.

[hpekristiansen]

You are wrong - there is not a thing you mention that is not available for non-planar sketches.

If a point is added outside of the sketch plane, the sketch is not planar. Fusion consider all sketches equal - all sketches are 3D, as I wrote. We humans can also not call the sketch planar or 2D - it is 3D or non-planar.

You are confused, because the mentioned functions are only available for sketch entities in the sketch plane. I will not participate in this thread anymore, as the OP questions has been answered.

[laughingcreek]

---

@hpekristiansen wrote:

...

All sketches are 3D in Fusion, in the sense that they can contain points in 3D.

Exactly.  All sketches have the potential to to be 3D.  They can be.

---

I was the only one answering OP's questions(as best as I could).

---

The very first thing the Op said was he was having trouble dimensioning.  Probably because his sketch was no longer 2d, but had become 3d.  Saying all sketches are 3d doesn't really help in understanding this nuance.

---

"within the context of how fusion works, there is a difference..." - really!!? Please explain this - maybe I am

wrong.

---

2d vs 3d sketch differences

Dimensioning is different.  constraints work different.  The way you define,move, and manipulate sketch elements is different.  Sketch patterns Don't work at all on 3d sketch elements. Tool choice will be different. Profiles are different (and yes, I know sketch elements of a profile just have to be planer, not necessarily on the sketch plane, but I'm not aware of any good work flows that use profiles that aren't on a sketch plane.)

Maybe it would be better to describe it as a "state".  Sketches are just sketches, they can exist in a 2d state, or a 3d state, depending on how you define the sketch elements. 

I agree the "3d sketch" checkbox is confusing.  I imagine  "allow snapping to 3d objects" would be more accurate, since you can still create 3d elements regardless of whether or not the box is checked.

[etfrench]

I have to agree with @hpekristiansen on this one.  Since a 2D sketch can contain 3D geometry even if the 3D toggle is not on, then the 2D sketch is in fact a 3D sketch.  Even if the 2D sketch does not contain 3D geometry, it can, therefore it's still a 3D sketch.

It would be better to just tell users which sketch operations are only available on geometry located on the sketch plane.  Being able to select sketch geometry and getting its properties would also help.

[Anonymous]

Thank you for your feedback.

I apologize but I can not send out the model as it is of unreleased product. If I delete previous features and bodies I am afraid the problematic sketch will not behave in the same way.

BR

Marco

[Anonymous]

Hi and thanks for your input.

I realize that at one point my sketch started snapping to geometries not coincident with the sketch plane. What I am interested in is why did this happened if I: 1 - specified sketch plane, 2 - unchecked "3D sketch" option in the sketch palette, 3 - unchecked "Allow 3D sketching of lines and splines" option in the Preferences/General/Design ?

But also I am not able to add any dimensions to the existing in the sketch geometry. If I add new elements however I can add dimension to those.

All these point to a non consistent behavior.

BR

Marco

[jeff_strater]

we are also interested in how this happened. As far as I know, the only two ways in which sketch geometry can be moved from the sketch plane are 

1. if the "3D sketch" option is on during curve (line/spline) creation, and you snap to model geometry
2. you use the Move command, while in sketch mode, select sketch geometry, and move it from the sketch plane (along the sketch Z axis)

If you can find and document another workflow that results in sketch geometry that is not on the sketch plane, we would like to see it.

you will not be able to dimension geometry that is not on the sketch plane.  Use the "Move to Sketch Plane" command to move that geometry back to the plane, and you will then be able to dimension it.

[Anonymous]

Hi Jeff,

I managed to reproduce the error and repeated it several times on two different machines with exactly the same outcome. I created a video to demonstrate the error. I have also isolated the relevant features and saved them to a new file I am attaching here.

video- https://autode.sk/35a5rDi

Thanks for your effort

Marco

[jeff_strater]

@Anonymous - thank you for the very thorough video and sample file.  That helps a lot.  I need to look at this a bit more closely, but it does seem like this behavior is a bug.  Very strange...  Thank you for taking the time to investigate this so thoroughly!

[laughingcreek]

@Anonymous - Did you by chance use "include 3d geometry" instead of the regular "project"?  That is how that projected line is behaving.

I can replicate your results with your model. But If I delete the original projected circle, and re-project using P for "projet", (and then reapply a coincident between the radial line and the newly created projection so everything turns black again), then making those edits work as expected.

[jeff_strater]

Thanks, @laughingcreek , I was wondering that as well.  But, I wanted to check internally if that was the case, because there is no UI that shows the difference between a Project and an Include.