Parameteric models using Conics and Splines

[dempseypj]

Ok, this is a mini-rant.

Please do not ask me to post files, they are all proprietary until I make a complete model to illustrate the problem.

Parametric modeling ALWAYS fails when using Conics or Splines. 2d and 3D sketches with conics and splines fail 100% of the time if any parameter is changed related to their positions.

I have basic parameters for an object that I need to fit around, so I have created the bounding box using parameters. These parameters are used to drive sketch dimensions. I create basic geometry and use conic curves for some of the corners to attempt to have some semblance of curvature continuity.

Basically, if I change ANY parameter, the sketch dimensions turn red and refuse to solve. The only solution is to delete the conic and re-sketch it. This, of course, is not acceptable as these are the control curves for lofts.

If there is anything with a tangent or curvature continuity in any sketch and and a parameter gets changed, the whole model fails to solve and requires a complete manual rebuild. I have noticed that all of the magical tutorials on the internet that show stuff like this working do not use conics or control point splines.

How am I supposed to make constraints so that parameters can be changed and still allow conics and control point splines to function properly?

Surfacing is a whole other problem that will need a separate post.

[Drewpan]

Hi,

I understand that your file is proprietary and you cannot post it, is it possible to see a partial screenshot?

Without seeing the actual issue, when the parameter change fails, what is the error message? Is it a red fail or a

yellow warning flag in the timeline? What happens if you click on the flag and edit the feature and when it opens

you simply click "ok" or close? Sometimes this will clear these flags. Have you tried direct value entry instead of a

parameter and does this fail? When you say "fail" CAN you fix it at all? How?

Your bounding box idea seems to be a good attempt to do what you need. It may be a simple fix or a bug or just not

the correct workflow. The forum will need a bit more information to help you.

Cheers

Andrew

[MichaelT_123]

Hi Mr DempseyPJ,

The sketch conic curve in F360 is, gently speaking … somewhat underdeveloped.

The troubles it causes are well documented on the Forum, e.g.

https://forums.autodesk.com/t5/fusion-design-validate-document/how-to-constrain-a-line-so-that-it-is...

… and you escalate the problem even further … by vogue, lacking precision in the description of your particular issue.

We (on this Forum) are Highly Intelligent, aren't we? But I would argue that you overestimate our capacity to give a specific answer to your call for help.

Nevertheless, I will shoot an arrow in a direction you might find promising in your project's context, which seems to be ‘conic-centric’. So ...

In 3D space, create a cone body, and intersect it with a construction plane. Both can be parameterized. Create a sketch based on the plane created and generate your perfect conic curve by a cone body intersection.

Let us know about the successes or failures of such an approach.  You can use a plain sheet of paper without the stamp ‘Highly Classified.”

Regards

MichaelT

[dempseypj]

Ok, I've made a quasi-representative model that I can share. The object and the geometry are highly dumbed down. I don't have all the lofts super clean.

The inability to make surfaces curvature continuous is very frustrating, tangent barely works. As you already know, tangents are not curvature continuous. Also, the "curvature continuity" sketch constraint just about never works, and it only works fit point spline to fit point spline under certain specific conditions. Fit point splines are basically terrible when you're trying to accurately control geometry.

During sketching, if you try to constrain a point to a specific point on a conic, good luck, it almost never stays ON the conic.

If I were to make a similar model in 3DX or CATIA V5, none of this would be a problem. If either of those options were actually affordable for any company that is funded < $100M, that would be nice. The workflow and most features of Fusion 360 are generally great. The major challenges are that Fusion 360, Solidworks, etc. are all geared towards SOLID Models, and I need to make parts with composite layups. There is an add on program for Solidworks to do this, but it requires Solidworks Premium and is also cost prohibitive. I wish Autodesk had not dropped their composites tools, they looked pretty good from what I can gather from the old documentation.

Feel free to play around with the model. Change any OBJECT dimension and everything breaks. The geometry does not stay affixed to the points, a tangent constraint or dimension breaks everything. You absolutely cannot rely on geometry in another sketch and have anything work. Without relying on the other geometry, it is impossible to properly constrain everything. Also, it is impossible to constrain everything because Fusion complains "the sketch is over constrained". There needs to be a way to pull up a table of constraints in a sketch, this is super simple to do. Fusion creates hidden constraints that you cannot get rid of that are breaking everything. If 3DX or CATIA V5 does this, you can pull up the constraints and figure out what the problem is.

I understand this is the "budget" product from Autodesk, and they want to push Inventor, RevIT, and other tools - which are worse for my application than Fusion.

I have to re-annotate my screen captures, apparently Windows didn't save the annotations. I'll attach them 3 at a time in subsequent messages.

Thank you very much for listening and taking the time to have a look!

Patrick

[g-andresen]

Hi,

An answer is not possible without insight into such a construction.
Share a sample file in which you recreate the situation.

günther

[dempseypj]

Here are a bunch of screen captures, sorry, they are out of order in the preview window here and I can't drag them around....

 

 

 

 

 

 

 

 

 

 

        

                

 

[dempseypj]

FYI, there is an attached sample posted 22 minutes prior to your post, not sure why you couldn't see it....

[Drewpan]

Hi,

Not wanting to state the obvious but if fusion complains about over constraining then you are constraining the

wrong thing. Have you tried the Text Command Sketch.ShowUnderconstrained? This will point out what points and

curves are unconstrained and helps greatly in nailing things down. While it is possible to constrain splines it isn't

easy and almost certainly would be the same as conics. Other points and curves are probably constrainable once you

have identified them.

Cheers

Andrew

[TrippyLighting]

I would stay away from conics in Fusion!

Very few people use them, and thus, you've likely discovered a few bugs.

I am running out of time today. I will see if I can get to the bottom of this over the next couple of days.

[laughingcreek]

It is completely true that fusion's sketch engine still needs some work.

I would also agree that conics are still probably buggy and might be best avoided.

but that said, I think a lot of this are unforced errors.  taking a different modeling approach will most likely elevate all the issues you are experiencing.

for instance, your first primary surface operation (loft1, not counting the helper bodies) violates 2 basic surfacing rules.

1-extrude, revolve, sweep, planner patch EVERYTHING that can be made with these operations before doing any lofts.  2-don't combine flat planner areas with curved loft sections.

(like all modeling rules, these are soft rules, and sometimes you absolutely want to do these things.  but not usually)

so the first loft-

can be changed to an extrude, which has the added benefit of providing cleaner, simpler underlying geometry to use for future operations, and eliminated the need for several additional sketches and surface operations.

I'm not completely sure of your design intent, but I suspect that you might even want to overbuild this surface and cut it back-

I'm hesitant to dig further.  if you want to step back and take a fresh approach (suggested) I'm sure you'll get lots of help.  based on my own experience, i don't see any reason why a parametric model that doesn't exabit all the various issues you're having can't be developed.

[TrippyLighting]

I agree that the lofting approach needs to be improved, but that isn't the reason stuff is breaking and that is also very easy to determine.

As the OP suggested, changing the value of Object_W from the "default" 200 to 210, for example,  breaks the sketch "CS1".

Completely unrelated dimensions turn red, and the sketch and plenty of following sketches and features break.

I've spent well over an hour trying to create a "CS1" sketch that doesn't use any construction geometry and no projections, and then the sketch updated just fine. Unfortunately, I had to add some construction geometry and an intersection point between one of the construction lines and a conic curve. That intersection point is used later in the design; if deleted, other sketches fail.

And then, magically, that super clean sketch also breaks when the aforementioned parameter is changed!

Conics are buggy, and this is just one of them. Also, the false errors Fusion provided me with while deconstructing and reconstructing that one sketch are disheartening, to say the very least.

Maybe someone else here has more luck tagging @Phil.E (the forum software is also buggy!)

It's AU time, and I don't expect an immediate response from anyone from AD right now 😉

[TrippyLighting]

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@Drewpan wrote:

Hi,

Not wanting to state the obvious but if fusion complains about over constraining then you are constraining the

wrong thing.

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Again, I have to challenge you to look at the design, spend some time with it, and find out what is really wrong BEFORE making general comments that don't really help anyone.

[Drewpan]

Hi @TrippyLighting 

While this design is way over my pay grade, my suggestion of the Text Command is still quite valid. It is not only

beginners who don't know about the command. I have posted previously and seen others recommend it to some

quite experienced people who didn't know about it and it helped solve the problem.

As you know, sometimes those couple of points that you missed are the problem and the command not only points

them out but allows you to see the local and sometimes big picture that puts them into context. I am not saying it is

the golden solution here. I made the suggestion to use it as a tool to help fix the issues. Removing the smaller issues

helps you see what the real problem is so you can concentrate on that.

Cheers

Andrew

[TrippyLighting]

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@Drewpan wrote:

Hi @TrippyLighting 

While this design is way over my pay grade,

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That's precisely why you need to sink your teeth into it and not let go until you've removed chunks!

That's how you learn ... and find bugs 😉

I have not used that text command in almost 10 years with Fusion. Never needed it!

The moment you need it, the sketch is too complicated, at least in Fusion.

[dempseypj]

I appreciate all the help everyone! Your insights are very helpful and well taken. Coming from CATIA V5 / 3DX is challenging. Figuring out how to accomplish simple tasks in those programs turns into a multi-hour scavenger hunt!

In CATIA, I would make a design table with all the parameters, a geometrical set that contains all the reference geometry, then create the conics all in another geometrical set - still ZERO sketches at this point, and then I would loft the surfaces. Sketches would be used for details farther down the line, especially sketches ON a curved surface for placing holes, components, etc.

In Fusion, the workflow requires creating many sketches and use 3D sketches to replace a geometrical set used for lofting. It is something to get used to.

I'll look at rebuilding with fewer lofts, and I agree that I could use extrude or sweep - I did in the original model that I cannot share.

Having a point constrained to the midpoint of the conic is required to get control of future guide rails that clean up the loft geometries - otherwise they balloon out instead of going to the correct place.

Thank you again for all the help!

Patrick

[TrippyLighting]

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@dempseypj wrote:

...

Having a point constrained to the midpoint of the conic is required to get control of future guide rails that clean up the loft geometries - otherwise they balloon out instead of going to the correct place.

....

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I have not actually tried to create "better" lofts in this particular design, but when lofts balloon out, often that is an indication that it should be broken into separate lofts/surfaces.

[johnsonshiue]

Hi! Certainly there is always room for improvement in Fusion Design environment in terms of modeling capability just as any design tool. But I personally think this model needs to be redone by starting from basic shape.

The issue with this model is that the detail geometry was taken into account too early. Blending, filleting should be done last, not first. To reverse-engineer a smooth model like this, one needs to remove those smooth curves and detail geometry. When a straight line or an arc can be used, do not use a spline. Only keep the smaller geometry if it is absolutely necessary and dimensionally critical.

Once detail geometry is removed, the original base shape is usually very simple.

Many thanks!

[dempseypj]

That may work if your primary goal is a solid model. There should really be very minimal blends or fillets in a surface model. Basically, a fillet should only happen where a wing attaches, it should be conic, and there should be a rule to make it more appropriate to the geometry. So, I should end up with three fillets that become mirrored.

I am also not reverse engineering anything, I'm trying to design an aircraft from scratch.

My goal is to create aerodynamic shapes that need to be tightly controlled, I have shared a simplified model to illustrate my points without providing the proprietary detailed geometry. Making a solid, highly manipulated block and then trying to hollow it out will not work. The shell command rarely works on complex geometry, and having dozens of "smoothing" operations is just asking for 100% breakage in your model - kind of like I'm experiencing now.

T-Spline shapes are generally curvature continuous by default, but the level of actual control you have is virtually non-existent. You can create a basic sketch to define the initial shape, but then everything else after that is not truly controlled and if you change the initial parameters, you shape gets wrecked.

There are plenty of RC Aircraft tutorials available, but the techniques used do not truly allow for a parametric model to be created. They meet the profile drawings that were used as a canvas, but if you needed to change something like the wing aspect ratio or twist, the model will break.

I can make a brick with simple geometry, but it will not perform well in the application.

[TrippyLighting]

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@johnsonshiue wrote:

...When a straight line or an arc can be used, do not use a spline. ...

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That is true for mechanical engineering modeling.

However, if yoo move on from IMHO simplistic solid modeling techniques into the area of industrial and product design you'll find that there are very few straight lines and arcs or circular fillets in such designs for good reasons.

Even the "simple" geometry of an iPhone, a rectangle with rounded corners uses few if any circular fillets!