Sketch constraints: Coincident or Colinear to Origin plane?

[Anonymous]

Folks,

Does anyone know if it is possible to constrain a line to an Origin (plane) in the Sketcher?  It would seem that you can only constrain a line-end point to be coincident with the Origin center point, the Sketch Constraints do not seem to allow one to use any of the linear parts of an Origin for constraining sketch entities.

If this is the case, I am wondering what purpose the Origin(s) in F360 actually serve the user.  If I can't dimension to it, can't align to it, can't use it as any sort of reference, then what does it do for me as a user at all?

I imagine there are some internal reasons for Origins, e.g. F360 wants seperate coordinate systems or something for bodies and components, but at the user level, what can one actually do with Origins?  In Solidworks Planes (essentially Origins) are eminently useful to the user, F360, I still can't figure it out.

Absent any sort of good comprehensive documenation for F360, I think it is these sort of fundamental UI/UX issues that should get top priority in the new builds.  How about fewer sugary new features and more rework of the core features that make the user experience so poor for those of us with years of experience on other large MCAD packages - I believe we are your largest audience. By core I mean things like these sorts of inconsistencies in the Sketcher, or the Model workspace (e.g. selecting from the top right vs lower left - what the heck?), or fixing the way X-ref'ed sub-assemblies can be configured and manipulated in a top level assembly, etc.

</rant>

[michallach81]

Hi,
I can't wrap my head around nature of your concerns. Nevertheless, first we need to be more specific. What do you mean by saying Origin? You're asking: "Does anyone know if it is possible to constrain a line to an Origin (plane) in the Sketcher?", and if you are asking is it possible to constraint sketch entity to a plane? Yes it is possible, even more it is applied by default, all your sketch entities are planar to chosen plane. Which mean they "sit" flat on a plane. Common request was to be able to break that relation, and Fusion team introduced 3D curve. If you have enabled that in your preferences, you can detach sketch entities from a plane. Is it possible to apply relation in third dimension? No, at least not yet, but to be honest it's not possible in majority of CAD softwares.
That was first type of geometry that creates Origin, a plane. As I said, there is only one relation applied, planar constraint. In theory we could have some 3D constraints, but believe me most of users would struggle to understand those relations and consequences of those.
Second type of geometry are axis, and unfortunadly we can't use them in sketch enviroment, we can utilize them only in modeling enviroment.

Third type of geometry is a point. We can apply many constraints with point of origin, like coincident:

Dimensions:

and we can use horizontal/vertical constraint:

There are few more option how we can use relations, but it depends on type of sketch entity we'll use.

In modeling enviroment we can utilize Origin mainly to align and to snap. Is it very different form other cad packages? Not much.

I have problem to understant other of your concerns, like type of selection. The way selection works is common in cad, and it's very handy. All those options like how we draw selection, filters, type of selection (box, paint etc.), all those you can find in other cad programs, and they works the same.

I'm not surprised that someone could have trouble to use assemblies in Fusion, mainly because here Fusion differs the most for other programs, and developers themselfs haven't yet figured out all off the aspects of that new system. I have to say that even with some flaws I like idea to work in single enviroment, being able to build and assembly in a same time.

[TrippyLighting]

The selection window in Fusion 360 works the same way the selection window has worked in Autocad for the last 25+ years.

dragging the window open from bottom left to top right selects only objects that fit compelely I the selectioon window 

dragging the window open from the top right selects all objects that are wholly or partially in the window.

[Anonymous]

Hi Trippy, Actually I was referring to a more complex behavior that surfaced in a previous post I made. The issue was, I had a sketch with several items that I wanted to extrude, and found that depending on the starting point and direction of the sketch, items from other sketches and geometry would be selected and extruded - not at all what I expected it wanted. The big problem is that behavior is not mentioned in the documentation anywhere, and coming from Solidworks, never having driven AutoCAD, I found it baffling. If starting point and direction make such a dramatic difference in the actions accomplished by the drag, it should at least be made clear to the user. I would argue however that this sort of modality is the bane of a consistent UI. Art

[Fully_Defined]

I totally agree with your original premise.

There are workarounds hiding in plain sight, EVERYWHERE, but for some reason Autodesk isn't trying to convert users away from Solidworks or any other platform by pointing them out. I have found myself, a Solidworks user, flabbergasted that Autodesk didn't think I would want to do something, but usually they just have a different way than Solidworks.

For example, I am designing a sailing yacht, and I want a spline on a waterline to terminate at the stern, at a specific distance from the centerline. The stern is at a specific angle from the horizon.

In Solidworks, going about setting up the plane the stern is on parametrically would have been a matter of inserting a plane perpendicular to the front plane and coincident with a line in a controlling sketch on the front plane.

In Fusion 360, it's an offset plane using the same line, however there is no reference to the front plane - it's implied by the sketch it's in. Selecting 90 degrees makes it perpendicular to the front plane. Parametrically that might be the weak point here.

So how do I make the spline terminus coincident with the stern, which is just a plane now? Well, YOU CAN'T, but by inserting a point coincident to three planes, including the one you just created and the plane the curve is sketched on, and then projecting that point, and then making that projected point horizontal/vertical with the terminus of the spline. Then dimensioning. Seems like a PIA, right? Well, IT IS.

What if I don't want projected points everywhere? Too bad!

And if - God forbid - you dimensioned the spline terminus instead of a point which you made coincident to it after the fact, then you are totally screwed if you reference your geometry later but change you mind about something upstream. It's possible to delete the coincident constraint to the point, but a terminus is a terminus is a terminus... if you delete it because you changed something you have to start over.

¯\_(ツ)_/¯

[GRSnyder]

Axes and planes in Fusion 360 are unbounded, a fact that Fusion 360 obscures by allowing you to project them into sketches as finite-looking line segments. Despite that, they are really more like the mathematical versions of lines and planes.

It's not meaningful to talk about the 2D projection of a plane that isn't perpendicular to the sketch plane, because the projection would cover the entire sketch. You can project origin planes and constrain against them, but only if they're perpendicular to the sketch, in which case they project as lines, just like axes. You may as well just project in the axes you want.

As @michallach81 says, if you want to constrain something to a plane, just sketch directly on that plane and project the geometry you want to constrain against into that sketch. If you want to constrain against two planes simultaneously, just construct the intersection line of those planes and project and constrain against that.

[Fully_Defined]

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@GRSnyder wrote:

Axes and planes in Fusion 360 are unbounded, a fact that Fusion 360 obscures by allowing you to project them into sketches as finite-looking line segments. Despite that, they are really more like the mathematical versions of lines and planes.

It's not meaningful to talk about the 2D projection of a plane that isn't perpendicular to the sketch plane, because the projection would cover the entire sketch. You can project origin planes and constrain against them, but only if they're perpendicular to the sketch, in which case they project as lines, just like axes. You may as well just project in the axes you want.

As @michallach81 says, if you want to constrain something to a plane, just sketch directly on that plane and project the geometry you want to constrain against into that sketch. If you want to constrain against two planes simultaneously, just construct the intersection line of those planes and project and constrain against that.

---

Enter the workarounds.

How about just relating to existing planes? Why is this prevented? You can justify it until you are blue in the face!

Here's the thing:

A boat has many parts that have predetermined dimensions on definable planes, and many parts that relate to them. Forcing my hand to project geometry is just forcing me to repeat functions I previously defined, and this is even more bitter because I can't just import predeterminded geometry within a design table. The result is errors stacked upon errors stacked upon errors, because there is no unified chain of command for geometry, because I have to stack projections.

If I were making a coffee table, we wouldn't be having this conversation.

[CruftMeister]

@Fully_Defined

Thanks for your followup post here, you have succeeded in making clear the point I tried but failed to make in my post.  At the time I posted I was just trying to use the datum planes (Origins in Fusion speak)  as I would in Solidworks or ProE, and didn't know about all the projection workaround stuff that Fusion needs.

<broken-record>

I just wish the Autodesk would make the Fusion sketcher operate more like the Solidworks sketcher . . .

</broken-record>

[TrippyLighting]

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@Fully_Defined wrote:
 

Enter the workarounds.

How about just relating to existing planes? Why is this prevented? You can justify it until you are blue in the face!

---

The workflow you prefer is not deliberately prevented, it just isn't implemented that way. If you can open your own thread, and share more details about your project we can probably point out other ways to accomplish what you want.

These other ways might be workarounds - Fusion 360 does have limitations -  or they might simply be different.

[kb9ydn]

I think the thing that frustrates Solidworks users when sketching in Fusion is that you can't directly reference any outside reference geometry without projecting it into the sketch first.  This may seem like a trivial extra step to have to do, but if you're used to having easy direct access to outside reference geometry from your sketches, it gets VERY tedious having to project that same reference geometry EVERY STINKING TIME YOU WANT TO USE IT.

One other place where you can't use reference geometry is with joints.  If you get into the habit of creating your components in such a way as to make the built in "origin" planes have some sort of meaning (like as center planes for the part or assembly), they become very useful and efficient alignment references, that you get automatically with almost zero effort.  Except that, oh wait, Fusion doesn't support that. 

C|

[GRSnyder]

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@kb9ydn wrote: I think the thing that frustrates Solidworks users when sketching in Fusion is that you can't directly reference any outside reference geometry without projecting it into the sketch first.

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It is indeed peculiar that Fusion 360 does not auto-project construction objects or origin objects even when "Auto-project edges on reference" is turned on. (The description of this option, in Preferences -> Design, is "Auto projects model edges to be used as a reference for creating constraints and dimensions in active sketch when orientation is normal to the active sketch plane.")

I wonder what the logic behind that design decision was. 

[kb9ydn]

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@GRSnyder wrote:

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@kb9ydn wrote: I think the thing that frustrates Solidworks users when sketching in Fusion is that you can't directly reference any outside reference geometry without projecting it into the sketch first.

---

It is indeed peculiar that Fusion 360 does not auto-project construction objects or origin objects even when "Auto-project edges on reference" is turned on. (The description of this option, in Preferences -> Design, is "Auto projects model edges to be used as a reference for creating constraints and dimensions in active sketch when orientation is normal to the active sketch plane.")

I wonder what the logic behind that design decision was. 

---

The simple answer is because it's limited to "model edges", but why this limitation I have no clue as it severely limits the usefulness of construction geometry.  But I would go a step further and ask, "why require projection at all"?  Why not just allow direct referencing and let the projection be implied?  That way the sketches aren't cluttered up with projected geometry everywhere.  If the software requires projection behind the scenes, that's fine, just don't put extra junk in my sketches.

C|

[GRSnyder]

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@kb9ydn wrote: But I would go a step further and ask, "why require projection at all"?  Why not just allow direct referencing and let the projection be implied?  That way the sketches aren't cluttered up with projected geometry everywhere.  If the software requires projection behind the scenes, that's fine, just don't put extra junk in my sketches.

That's not clutter; it's important and useful information.

I would imagine the main motivation behind this design is to make it easier to diagnose and fix problems when the design changes and breaks the projection. In that case, the sketch is marked as broken and you can open it and see, ah, yes, that projected line that you constrained against is the thing that no longer exists.

This type of breakage is pretty common, so there's potentially some value in requiring projections to be explicit. "Yes, I acknowledge that I'm adding a dependency on something outside this sketch."

I suppose you could still display error projections even if projections were normally implicit and hidden, but it would be a bit strange to have new geometry appearing in your sketches when they broke. How does SolidWorks handle this case?

A couple of other potential benefits of explicit projections:

1) Even in the absence of errors, it's nice to be able to audit a sketch to see what the relationships are. If you hover over, e.g., a parallel constraint icon, it highlights the two lines that are parallel. 

2) Similarly, many constraints are symmetric. It's nice to be able to ask not only "what reference object is this line parallel to?" but also "what are all the objects that are parallel to the X axis?"

For both #1 and #2, I suppose you could start highlighting and constraint-annotating objects outside the sketch to recover these abilities, but that does sound kind of messy. It's nice that Fusion currently maintains a pretty clear distinction between what is and is not a part of a sketch.

3) Things don't always project in their original form. Lines may project as points, planes project as lines, curved faces project as profiles, etc. This distinction is important because the constraint system is 2D. You  really are constraining against 2D projections, which may be quite different from their source objects. Explicit projections show these transformations directly and unambiguously.

4) You can't get rid of the ability to explicitly project geometry; it's too useful. Given that you have this feature, and that it's sufficient to support the types of relationships discussed in this thread, the bar is pretty high for adding a separate, parallel system that is kinda sorta exactly like projected geometry but with its own set of behaviors and visibility rules. There would need to be a significant drawback to projection or a significant benefit to a new system to justify it. 

There's always room for improvement, but the current system is simple, elegant, and consistent. Every design choice is a tradeoff.

[Fully_Defined]

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@GRSnyder wrote:

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@kb9ydn wrote: But I would go a step further and ask, "why require projection at all"?  Why not just allow direct referencing and let the projection be implied?  That way the sketches aren't cluttered up with projected geometry everywhere.  If the software requires projection behind the scenes, that's fine, just don't put extra junk in my sketches.

That's not clutter; it's important and useful information.

I would imagine the main motivation behind this design is to make it easier to diagnose and fix problems when the design changes and breaks the projection. In that case, the sketch is marked as broken and you can open it and see, ah, yes, that projected line that you constrained against is the thing that no longer exists.

This type of breakage is pretty common, so there's potentially some value in requiring projections to be explicit. "Yes, I acknowledge that I'm adding a dependency on something outside this sketch."

I suppose you could still display error projections even if projections were normally implicit and hidden, but it would be a bit strange to have new geometry appearing in your sketches when they broke. How does SolidWorks handle this case?

A couple of other potential benefits of explicit projections:

1) Even in the absence of errors, it's nice to be able to audit a sketch to see what the relationships are. If you hover over, e.g., a parallel constraint icon, it highlights the two lines that are parallel. 

2) Similarly, many constraints are symmetric. It's nice to be able to ask not only "what reference object is this line parallel to?" but also "what are all the objects that are parallel to the X axis?"

For both #1 and #2, I suppose you could start highlighting and constraint-annotating objects outside the sketch to recover these abilities, but that does sound kind of messy. It's nice that Fusion currently maintains a pretty clear distinction between what is and is not a part of a sketch.

3) Things don't always project in their original form. Lines may project as points, planes project as lines, curved faces project as profiles, etc. This distinction is important because the constraint system is 2D. You  really are constraining against 2D projections, which may be quite different from their source objects. Explicit projections show these transformations directly and unambiguously.

4) You can't get rid of the ability to explicitly project geometry; it's too useful. Given that you have this feature, and that it's sufficient to support the types of relationships discussed in this thread, the bar is pretty high for adding a separate, parallel system that is kinda sorta exactly like projected geometry but with its own set of behaviors and visibility rules. There would need to be a significant drawback to projection or a significant benefit to a new system to justify it. 

There's always room for improvement, but the current system is simple, elegant, and consistent. Every design choice is a tradeoff.

---

I'm not discounting your obvious passion and thoughfulness on this topic, but I disagree.

Fair enough, you want projected lines. I don't. Let me have that option. Let me constrain to planes! You know what would also be nice? Being allowed to trim projected lines, splines or curves! I don't know how to do that in Fusion.

If I were making a coffee table, I probably wouldn't need many planes or projections.

How about a wooden sailing yacht though? I want to have at least 60 planes, and have hundreds (HUNDREDS!) of points at predetermined coordinates, with two of the points' axes COINCIDENT WITH PLANES. Each of these points become coincident to spline fit points, and this spline then feeds an intersection curve. Multiply that several times and it starts to fill up with superfluous purple lines and repetitive clicking, and it starts to get pretty ugly on screen.

In order to do accomplish my mission in Fusion, I added parameters that match the distances from the origin that the planes would have existed at, and then used that parameter as the dimension when placing the points. It allowed me to get some consistency without seeing red dots everywhere even when the sketch isn't open. But it's a workaround, and not ideal.

Also, don't put so much faith in projected geometry when it is totally hidden behind a stack of points! If the frontmost entity is black, the purple projected geometry is hidden. Because Fusion hides sketch relations, I have no idea what a given sketch entity is related to until I hover over it and long left click. That is just absurd when I have hundreds of points in a sketch with relations. In Solidworks, I get a little green box next the point, and if I click something I can see what the relations are and delete or modify them at will. Not so in Fusion.

[TrippyLighting]

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@Fully_Defined wrote:

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How about a wooden sailing yacht though? I want to have at least 60 planes, and have hundreds (HUNDREDS!) of points at predetermined coordinates, with two of the points' axes COINCIDENT WITH PLANES. Each of these points become coincident to spline fit points, and this spline then feeds an intersection curve. Multiply that several times and it starts to fill up with superfluous purple lines and repetitive clicking, and it starts to get pretty ugly on screen.

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Please start a separate thread and share at least some screenshots.

It sounds to me that you are creating a framework for a boat with way too many spline points and way too many rails.

If you want to loft this then that won't result in what you are hoping for.

[Fully_Defined]

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@TrippyLighting wrote:

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@Fully_Defined wrote:

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How about a wooden sailing yacht though? I want to have at least 60 planes, and have hundreds (HUNDREDS!) of points at predetermined coordinates, with two of the points' axes COINCIDENT WITH PLANES. Each of these points become coincident to spline fit points, and this spline then feeds an intersection curve. Multiply that several times and it starts to fill up with superfluous purple lines and repetitive clicking, and it starts to get pretty ugly on screen.

---

Please start a separate thread and share at least some screenshots.

It sounds to me that you are creating a framework for a boat with way too many spline points and way too many rails.

If you want to loft this then that won't result in what you are hoping for.

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Hoping for?

I already did it, dude.

Here is a sketch with what seems to work best in Fusion 360. There are only two points in this sketch that I want to project; one of them is an intersect project and the other is a point on another sketch. The dimensions that are parameterized are where the planes should be (but aren't), and so the points should really be just coincident to planes. I shouldn't have to dimension them for every water line, and I don't want projected points in the sketch.

Everything in this sketch is dimensioned from the origin.

In Solidworks, I would have been done with the entire skeleton by the time I had finished this post.

[TrippyLighting]

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@Fully_Defined wrote:

Hoping for?

I already did it, dude.

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If you used hundreds of points as spline fit points to create the rails and profiles for a boat then you certainly can loft geometry rom that, but I would urge you to use the curvature comb, the zebra stripe tool and the curvature map to inspect your results and see if you are happy with it.

Fit point splines in Fusion 360 are 5-degree multi span splines and with too many control points the geometry created from such curves is usually pretty bad.

It is also entirely possible that I have misinterpreted your design method used on too little information. Thus the request for a new thread 😉

[GRSnyder]

Well, if you're dead set on avoiding all interactions among sketches or planes, then you've reduced the problem to "How do I create a spline from data points without having to dimension everything by hand?"

Just import the points and lock them in place.

[Fully_Defined]

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@GRSnyder wrote:

Well, if you're dead set on avoiding all interactions among sketches or planes, then you've reduced the problem to "How do create a spline from data points without having to dimension everything by hand?"

Just import the points and lock them in place.

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Alright, now we're talking.

I have until this moment thought it was impossible to import design tables. Where did you get that script?

If I change my mind on a dimension from that table, but I have already used that spline in an intersection curve, which itself was used downstream, does my model blow up? It seems like this is what scares me the most about Fusion 360.

[GRSnyder]

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@Fully_Defined wrote: I have until this moment thought it was impossible to import design tables. Where did you get that script?

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I'll sell you a copy for $500! 

I think it's part of the default examples. But if not, attached.

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If I change my mind on a dimension from that table, but I have already used that spline in an intersection curve, which itself was used downstream, does my model blow up? It seems like this is what scares me the most about Fusion 360.

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You can edit without breaking anything. For example, you can tweak the location of a particular point by selecting it and using the Move command.

If you have to reimport the entire dataset, that generates a new spline (and a new sketch, as the script currently does it); the associations won't be maintained. However, if you are just generating a surface and using that surface in a later intersection operation, you can retarget the existing intersection operation to include the replacement surface instead. Nothing downstream of that should be affected.