Sketch constraints: Coincident or Colinear to Origin plane?

[CadZebra]

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>

[TrippyLighting]

@GRSnyder your screencast is missing the application of a curvature comb.

[kb9ydn]

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@GRSnyder wrote:

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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?

 

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As far as explicitly showing referenced outside geometry as projections in the sketch, I would agree that it's going to be a matter of preference.  I prefer implicit and hidden mostly because it's what I'm used to.  So ideally it would just be a setting that you can click on or off, e.g. "show outside referenced geometry in sketch", or some such.  This doesn't really bother me that much.  What bothers me much more is having to go through a separate step where I have to manually project some outside reference plane/line/point into a sketch, just to dimension or constrain to it.  In this instance reference geometry should not be treated differently than other model geometry.

So how does Solidworks show broken references?  Any sketch entities that have broken references will change color, and the dimension or the constraint icon will change to the same color.

With broken dimensions, if you click on the dimension it will show a red dot at the point where the extension line meets the formerly referenced thing, and if the referenced thing is out of plane with the sketch it will show a ghosted line of the referenced thing, to give some idea of what it was.  The ghosted missing entity is somewhat hit or miss though.  It will sometimes show and sometimes not.  To fix it you can either delete and recreate the dimension or you can click and drag the red dot to somewhere else to establish a new link.

For broken sketch constraints it basically the same thing, except now you can double click the constraint icon and bring up a window where you can see which referenced entity is missing and link in something else.

Being able to re-link broken references is something that Fusion sorely needs.  I'm sure someday it will get there.

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@GRSnyder wrote:

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 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.

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#1 is pretty much exactly the same in Solidworks, except that for things outside of the sketch it highlights the thing you referenced instead of a projection of that thing.  To me this is preferable because it shows the actual source.

#2 I'm not sure I follow what you mean.

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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.

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Actually the constraint system in Fusion is not 2D.  You can apply constraints to out-of-plane model geometry and it will move your entities off the active sketch plane.  I think you may have to have the "Allow 3D sketching..." option checked for this.

Interestingly though, Solidworks sketching IS normally 2D by default, so when you reference outside things you are always referencing a 2D projection.  This is just something that is assumed and known.  You can also sketch in true 3D mode, but that's a completely different animal with it different set of constraint rules than 2D sketching.  I try to avoid it unless absolutely necessary, as it can get really complicated in a hurry.

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@GRSnyder wrote:

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.

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I wouldn't get rid of explicit projection.  In some cases it's required, and I use the equivalent function in Solidworks all the time.  It's just that I only use it where the resulting line/arc/etc. will be used directly for geometry creation.  If it's only being referenced by a dimension or constraint, then I don't want to see it.

What Fusion has now is fine for the most part, it just needs a few adjustments:

First; treat reference planes/lines/points the same as direct model geometry, so they can be used directly in sketches for dimension/constraints, and in joints (this is the biggest one).

Second; allow a bit more visibility control for how/when projected entities are displayed. (nice to have but, could live without it)

And really it's as simple as that.

C|

[Fully_Defined]

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@TrippyLighting wrote:

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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 😉

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I have zero plans to loft anything. This will be a patch, with curves as interior rails; the curves will be created from intersection projects on planes strung along the centerline. Again, stuff Fusion 360 doesn't allow so I have to get creative.

Lemme give you some background. There is a well-known boat from 1909 that is being restored on a YouTube channel I won't name here. The vessel was wrecked in the 1960s and cobbled back together, and then spent a couple of decades rotting away on dry land. Landlubbers, AMIRIGHT?

The original plans still exist in high resolution scans; in fact all of the original drawings are available. I started to create a digital model on Solidworks, but then I remembered that I could share projects (for example, with the guy whose project this is - it's not mine!) on Fusion 360, and that's why I even care.

An unsung marquis feature of Fusion 360 is scaling canvases. For some reason, this is not possible in Solidworks, and makes what I am doing very difficult. Here in Fusion 360, I have a controlling sketch with points taken directly from the plans from 1909. 

So here's the thing: I was invited to participate in Solidworks' new Fusion 360 killer beta, xDesign. I like what I see! I also have a soft spot for Autodesk, and I want to see them succeed... I just need to relate sketch entities to planes. If they can't give that to me, what am I supposed to do?

[TrippyLighting]

I took the sketch with the spline and re-created it with out the end points as they are projected from somewhere else and don't carry dimension. It does not matter for what the image below demonstrates.

Whatever method you use to create a surface, if you use this spline to create the surface, the curvature of that surface will be the same terrible quality as shown in the image. It matters not if that curve was created by mathematical means and then is imported per script. Unless the method that creates the spline also uses a 5-degree multi span spline and the imported points are exactly the spline fit points then the curvature is going to be terrible. There's no way around the math here.

The actual surface quality might in the end of no concern for a manually manufactured boat, however you'll have to get to that point first. These curved surfaces, are often just the basis for further work and they might be trimmed etc. With such curvature these trimming operation will create broken edges and that in itself might prevent a project form completion.

@Fully_Defined I agree, this is a cool project.!

[michallach81]

Don't bother yourself Peter, there's no way to convince "those who know better".

[Fully_Defined]

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@TrippyLighting wrote:

I took the sketch with the spline and re-created it with out the end points as they are projected from somewhere else and don't carry dimension. It does not matter for what the image below demonstrates.

Whatever method you use to create a surface, if you use this spline to create the surface, the curvature of that surface will be the same terrible quality as shown in the image. It matters not if that curve was created by mathematical means and then is imported per script. Unless the method that creates the spline also uses a 5-degree multi span spline and the imported points are exactly the spline fit points then the curvature is going to be terrible. There's no way around the math here.

The actual surface quality might in the end of no concern for a manually manufactured boat, however you'll have to get to that point first. These curved surfaces, are often just the basis for further work and they might be trimmed etc. With such curvature these trimming operation will create broken edges and that in itself might prevent a project form completion.

@Fully_Defined I agree, this is a cool project.!

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All of the values you see were recorded by a man with a tape measure in 1909, and there's a lot more where that came from. Of course they're off! The whole point of all of this is to fair the lines so they are graceful and more hydrodynamic. I have to start with a skeleton that I can then alter, and all of this madness with repeatedly entering identical values just to avoid having sketches with 10,000 purple lines with relations I can't see is starting to make me rethink using Fusion 360 for this project.

That leads me to why I hate going on forums. While I believe all of you have your hearts in the right place, you make far too many assumptions about people like me who go on places like this to engage in technical discussions. I always end up with people trying to convince me I don't know what I'm talking about. Smarter people than me might take that as a hint, but I'm too stubborn!

[TrippyLighting]

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@michallach81 wrote:

Don't bother yourself Peter, there's no way to convince "those who know better".

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Agreed!

[michallach81]

@TrippyLighting I don't know if vintagerider will alter his design, but he will alter arguments, for sure.

@Fully_Defined It doesn't matter if measurements were made in 1909 with a tape. In 1909 they've expressed they intent directly in a model, and sections were drawn off of it.

You are in a different position, using MCAD type of software we expressing intent with sketches, but those old sections drawings are useless since they weren't used to define the shape.

Hull is a very specific "organic" shape and with few exceptions, it's almost impossible to imagine shape through sections, relations between sections are to complex for humans perception.

Even simple surface modeling is not enough (in most cases), to define a complex shape.

The most common way in modern days is to sculpt NURBS:

or sculpt some sub-d (like t-splines):

Since I'm true a$$hole I'll share with you few modeling tips from actual ship designers:

http://aerohydro.com/marinesupport/docs/ClassicHulls/modeling_classic_sailing_yacht_hulls.pdf

http://aerohydro.com/marinesupport/docs/ship_hulls.pdf

and more from them:

http://aerohydro.com/?page_id=979

I know it's all in different software, but I will grant you that you're PRO so you won't have any problems to utilize those in Fusion, as I did:

We know that you know all of that already,  we just waiting for your sophisticated argument why you've made that keel line so dense and fully constrained.

[lichtzeichenanlage]

This discussion with will not end nicely...

[michallach81]

True it won't... @Fully_Defined is struggling with just a hull design.

His elaborated workflow will let him create this walnut texture:

but even this failure he could execute only in Solidworks, in Fusion he will even fail to fail.

I'm actually helping him, but he won't see that, I've accepted that.

[Fully_Defined]

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@michallach81 wrote:

True it won't... @Fully_Defined is struggling with just a hull design.

His elaborated workflow will let him create this walnut texture:

but even this failure he could execute only in Solidworks, in Fusion he will even fail to fail.

I'm actually helping him, but he won't see that, I've accepted that.

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Oh, what the hell, I'll take the bait!

1) I have never claimed to be a ship designer - amateur or professional.

2) I have a specific data set that already exists. I AM NOT DESIGNING ANYTHING.

3) I am already done with what we are talking about, in Solidworks. I was duplicating my work in Fusion so I could share it.

4) Thank you for sharing your links. All help is appreciated.

5) You are basically proving my earlier point about forums. It feels like I am lost in the wrong neighborhood.

[PhilProcarioJr]

@michallach81

I think you guys are missing the point that @Fully_Defined was/is trying to make. From everything I have read that he posted he never intended to make a model of the boat but rather needed a way to convey current information to a group of people that may or may not intend to make a model. He stated that this design was of a boat made in the past and not one of his own design. Although you guys are right that the data that @Fully_Defined has can not be used in it's current form to produce a good CAD model, you missed the fact that it was not his intent.

The points he brings up about the differences in projections between Fusion 360 and Solidworks are very valid points and one of the things that drives me nuts about Fusion. Projections are broken in Fusion and need a lot of TLC. The way they work is passable at best and annoying. There is nothing worse then a bunch of useless information and broken elements in a sketch...

Just my 2 cents.

[CruftMeister]

Phil,

Thanks for weighing in and summarizing.  I completely agree, the current projections in Fusion drive me nuts too, and yes, a lot of TLC is needed there.  Fusion has some very powerful capabilities, but there are also some glaring flaws that seem to remain year after year, which is too bad. . . 

[TrippyLighting]

@PhilProcarioJr 

"I have zero plans to loft anything. This will be a patch, with curves as interior rails; the curves will be created from intersection projects on planes strung along the centerline. Again, stuff Fusion 360 doesn't allow so I have to get creative."

I would interpret that as trying to skin a surface, which is not an unusual workflow to create the hull of a boat.

I did ask to take this to a different thread because it has noting to do with the sketch deficiencies discussed in this thread. That would have been an easy way to clarify, discuss and document and exchange experiences, which would also serve as a good reference with those that might want to create a physical model of the boat.

I don't recall making any recent references in this thread to the sketching/projection problems discussed here but ...

Yes, I agree that some of the functionality would be very useful. The ability to constrain a sketch point to a construction plane would be very helpful and vice versa, the ability to constrain a construction plane to a sketch point.

Having to project everything you want to use in a sketch into that sketch is really frustrating in more complex designs and then points are stacked on top of points and more points. They are only listed in that puny little hold-mouse-button window that does not allow for much interaction. Or you start making even more sketches.

The point (pun intended) is, however that Fusion 360 relies way too much - almost exclusively - on such an outdated concept as sketching. But so are so many users that come from other CAD applications.

We should really not be discussing how to improve the sketch engine. If we really want to move the tools ahead, we should be discussing how model without sketching! As it pertains to Fusion 360 I am not hopeful we'll get to that level. As such I must say that discussions about limitations of the sketch engine in Fusion 360 have started to get boring.

[kb9ydn]

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@TrippyLighting wrote:The point (pun intended) is, however that Fusion 360 relies way too much - almost exclusively - on such an outdated concept as sketching. But so are so many users that come from other CAD applications.

We should really not be discussing how to improve the sketch engine. If we really want to move the tools ahead, we should be discussing how model without sketching! As it pertains to Fusion 360 I am not hopeful we'll get to that level. As such I must say that discussions about limitations of the sketch engine in Fusion 360 have started to get boring.

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Indeed!  And I would say that the reliance on having to always project reference geometry into 2D sketches is one of the things that holds Fusion back.  2D sketches are certainly useful and they have their place, but generally they should be used only as the most basic framework possible to get to a 3D form.  Then the real modelling can begin.

C|

[GRSnyder]

@michallach81, that kayak model gives me hope for humanity...

Are you at liberty to post the model file? I would be interested in studying it.

[Fully_Defined]

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@GRSnyder wrote:

@michallach81, that kayak model gives me hope for humanity...

Are you at liberty to post the model file? I would be interested in studying it.

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Sorry, no. Honestly I should not have even posted the previous data, but the cat's out of the bag.

I went back to Solidworks for this project, and BTW - Solidworks isn't perfect either. I cut my teeth on Fusion several years ago, and I still prefer it for CAM over CamWorks.

[GRSnyder]

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@Fully_Defined wrote:

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Sorry, no. Honestly I should not have even posted the previous data, but the cat's out of the bag.

Oops, sorry I wasn't clear - I was wondering about @michallach81's kayak model.

[michallach81]

Sure thing depicted model still require to be re-topologized on front and rear hatch, but this model served only to evaluate eventual manufacture.

[michallach81]

"From everything I have read that he posted he never intended to make a model of the boat".

He didn't, Phil ???

@Fully_Defined:

"For example, I am designing a sailing yacht..."

@TrippyLighting:

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

@Fully_Defined:

"Hoping for?

I already did it, dude."

English is a foreign language for me, but I'm not stupid. I take an offense on that Phil.

As I told Peter, our friend will just alter his arguments.

Phil, be honest, how anyone could come to such idea:

"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."

@Fully_Defined is not in a position to judge, his points are mere speculations.