Constraining 3d vs 2D sketches

[fsonnichsen]

I am a bit confused on Sketch constraints. I note that I can fully constrain a sketch by confining only 2 of the Cartesian coordinates. Thus is I set distances from the origin for X and Z the sketch can be fully constrained (after constraining its component parts).  Seems like the 3rd axis is forgotten here.

  This would make sense in a 2D world but I vaguely get the impression that we are dealing with 3D for fusion sketches. In fact I can twirl the sketch about showing the 3d axis and further, I can apply the copy/move to move the sketch along this axis. When I do this the "lock" for fully constrained disappears--almost as if it implies that we have moved from a 2D to a 3D world. 

   What is worse I cannot seem to re- constrain the sketch for 3D at this point. 

What am I missing here?

Thanks

fritz

[Haad_Ali]

@fsonnichsen I think so the constraints do not seem to work in the 3D sketch. The same thing I have to face during my last time except for the straight lines along 3 axes.

[shahriarsifat1802164]

Hi,
When your sketch gets fully constrained the whole sketch gets black in color for (2D).
For a 3D sketch draw the sketch on the required plane and give relation and dimensions.

Fully Constrained sketch 

Thank you.

[TrippyLighting]

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@shahriarsifat1802164 wrote:

...
For a 3D sketch draw the sketch on the required plane and give relation and dimensions.

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Wouldn't the purpose of a 3D sketch be not to be constrained to a plane?

[fsonnichsen]

Thanks all for the replies.

I think the points made are true but  I still think something is missing. As Trippylighting says the confinement of a sketch to any plane, x=1,y=1,z=1 for example, is still just a 2D sketch after all. My issue is that I don't see whey a 3D sketch cannot be confined and I would think it may need to be. Perhaps they are no longer considered to be a sketch at that point-something of half way between a solid and a sketch. After all I don't think that in Fusion, a sketch can become part of a design on its own--even a plane sheet of metal has some small dimension in all 3 planes. 

  Think of orthoscopic projection in a set of engineering drawings--a 3D object is reduced to three 2D drawings. Perhaps it is the intent that fusion works that way but I have never seen it stated.

  If I want to move an object on a 2D sketch to the 3rd dimension, I must first remove the constraints. At that point it does not re-constrain.  Probably the need for 3D constrained sketching is not needed.

     If you want to Sweep a line and a circle for example the line must intercept the circle. If they do not you can still sweep but you get an error. But one can use the "Construct: Plane along a path" to circumvent this problem. This creates a plane at the end of the line. 

  So perhaps I am suggesting something that is never used. These are things that would save a lot of time if Fusion had written documentation deliberating on them--I think they are important to understanding how Fusion is to operate.

Thanks all

Fritz

[TheCADWhisperer]

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@fsonnichsen wrote:

 So perhaps I am suggesting something that is never used. These are things that would save a lot of time if Fusion had written documentation deliberating on them--

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I am surprised that @jeff_strater has not jumped in here, but at the risk of muddying the waters - 

- other parametric MCAD softwares like Autodesk Inventor permit fully defined 3D sketches.  They also have two distinct sketching environments 2D and 3D.

It is my understanding that in the beginning (of Fusion) that all sketches would technically be "3D sketches" even if confined to a plane.  In the beginning - it was not possible to fully constrain a sketch.  Over they years I have noticed a transition in Fusion away from "Design Differently" to "Design like in Inventor (and SolidWorks)".  A 3D toggle was added to the Sketch Palette in fairly recent times, but full parametric control still not developed.

Having said that, nearly all (but not all) of my 3D sketching (in any parametric MCAD software) is actually projected intersections of 2D sketches or at least controlled by 2D sketches - so all editing of my 3D sketches (after projection) is done in the 2D sketches.

Well, I am sure I have muddied things up, so hopefully @jeff_strater will come along and clear up the 3D sketch topic as it stands today in Fusion.

[TrippyLighting]

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@TheCADWhisperer wrote:

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@fsonnichsen wrote:

 So perhaps I am suggesting something that is never used. These are things that would save a lot of time if Fusion had written documentation deliberating on them--

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I am surprised that @jeff_strater has not jumped in here, but at the risk of muddying the waters - 

- other parametric MCAD softwares like Autodesk Inventor permit fully defined 3D sketches.  They also have two distinct sketching environments 2D and 3D.

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Yep, and as you know, there's a reason for that! The use of 3D sketches is mostly limited to specific use cases.

As it pertains to engineering disciplines this applies for example to frames, or piping, hosing, wiring etc.

A lot of people use 3D sketches when they should not and when it also isn't really necessary. As most Fusion 360 tutorials are made by other hobbyists without much history in CAD or 3D modeling, bad techniques proliferate quickly throughout the community. That isn't limited to sketching as we both have experienced in a number of threads where people have referenced YouTube tutorials that used questionable techniques.

[jeff_strater · Accepted solution]

Sorry, email notifications have been down for over a week, they just came back today.  I rely on that completely, so I missed this (and doubtless countless other important threads).  Thanks for the ping today, @TheCADWhisperer . 

At the risk of way more information than you may want, here is a bit about the history and philosophy of sketches in Fusion.  As you may know, Fusion uses a different sketch solver than Inventor/Solidworks/Onshape/everyone else on the planet.  That has its downsides, as @TheCADWhisperer and @TrippyLighting will tell you as long as you are willing to listen.  But, there is one upside:  Fusion's solver can handle 2D and 3D at the same time.  So yes, Fusion's sketches are all inherently 3D.  (BTW, labeling that check box in the palette as "3D" is misleading - all that setting does is change the behavior of the creation commands, to let you snap to 3D geometry.  That's another battle that I lost...)  So, yes, all sketches contain 3D geometry.  However, geometry that is on the sketch plane is treated specially.  You can think of sketch plane geometry as having kind of a soft constraint to the sketch plane.  That is why sketch plane geometry can be fully constrained with just 2D dimensions - the sketch plane constraint is restricting its motion in the sketch Z direction.  That constraint can be broken with the Move command, then that geometry can be moved anywhere in 3D space.

3D sketch geometry CAN be fully constrained.  It is just a bit harder, due to missing constraints.  Here are some examples of fully constrained 3D sketch lines:

But, it can be hard to fully constrain a 3D sketch curve - you can get there with dimensions:

we plan to add more 3D constraints and dimensions going forward.

[fsonnichsen · Accepted solution]

Thanks Jeff. There is never too much information for these things (and why I wish there was more written documentation).

I think this statement by you clarifies a lot of my confusion:

"That is why sketch plane geometry can be fully constrained with just 2D dimensions - the sketch plane constraint is restricting its motion in the sketch Z direction. That constraint CAN BE BROKEN with the Move command"

That is not immediately obvious and I came to a similar conclusion playing around with the move command. I had a construct of two sketches in two different (orthogonal) planes. I wanted one to touch the other which mandated moving by translating its plane. It still was 2D -e.g. all in one plane--but had a sort of "phantom" 3rd dimension so I could move its plane. I think the key is to design constructs where things meet properly to begin with.

One final note--the MOVE command and what it does to sketches, bodies, components etc is probably critical and fundamental to understanding fusion but again there is no good doc deliberating on this. I still am not clear on a lot of things about it and will need to resort to trail and error to learn more.

Thanks again for your post

Fritz