Cannot get my sketch to become fully defined (sketch made with splines)

[Justine_makes_things]

Hi,

First of all forgive my horribel sketch. I come from a Blender background and I'm still learning how to use Fusion and the parametric modeling workflow.

I'm trying to make a profile shape based off a reference image. I calibrated the refrence image so I know my proportions are correct. Now I can't get my sketch to become fully defined so I can cut out a square in the middle. 

I read on these forums that the spline handle dimensions need to be defined, which I did. It looks horrible and ugly, I know.

I defined the angle between the normal straight lines and the spline lines.

I constrained the length of the object with a construction line which dimension I also defined.

I don't know what else I can constrain/define to get my sketch to become fully defined.

Thanks in advance for any help! And sorry if this question is quite beginner level. I'm trying to get the hang of it.

 

[g-andresen]

Hi,

1. splines (especially fit-point splines) are difficult to determine completely and do not have to be.
It is only important to use as few control points as possible.
2. for such constructions, you should only sketch one half, extrude it and then mirror the body.
3. the horizontal alignment of the lower construction line is important.

Please share the file
File > export > save as f3d locally > attach to post

günther

[Justine_makes_things]

Hi Gunter,

Thank you for replying. I reattached the file to my initial post. Something must have gone wrong the first time around.

Mirroring is not really an option because the profile is not completely symmetrical. There's a very subtle yet important difference between the left and right side.

If I constrain the lower construction line to be horizontal then my sketch would be fully defined?

How would you go about modeling this shape if not with splines?

[g-andresen]

Hi,

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@Justine_makes_things wrote:

If I constrain the lower construction line to be horizontal then my sketch would be fully defined?

How would you go about modeling this shape if not with splines?

---

1. that alone will not be enough.
2. without splines I wouldn't do it either, although I would prefer a "control point spline".

But that requires a certain familiarity with it.

As the canvases are not implemented, it is unfortunately not possible for me to check the geometry.
Therefore, I cannot check the alignment and position of the construction line and possibly align the canvas.
However, as I have already mentioned, the number of control points should be reduced in order to achieve a more harmonious curve. The shape of the curve can then be optimized by repositioning the remaining control points and adjusting their tangents in length and slope.
Perhaps you can upload the canvases as separate images.

günther

[TrippyLighting · Accepted solution]

If you want to replicate an existing shape, please attach photos from different angles.

I am somewhat convinced that extrusion from a spline-based profile isn't going to capture the shape properly.

Scratch that, I somehow scrolled past the image.

5 arcs capture the top of the shape perfectly well. 2 for the bottom.

Of course the sketch engine does not recognize the bottom arcs as fully constrained when they are.

The overall canvas scaling was based on a 150 mm ballparked maximum width.

[g-andresen]

Hi Peter,

I have the canvas in the browser, but no content in the frame on the desktop.
Do you have any idea why this might be?

günther

[Justine_makes_things]

Hi @TrippyLighting Peter,

Thanks for taking your time and redoing the profile shape. It looks much better and cleaner. What did you use for the curves? Is there a way to trace through your sketch steps with fusion 360? It would make a great learning opportunity. However, the sketch is still not fully defined? Do you know the reason for this? I need it to be fully defined so I can make a new sketch on the extruded top side of the the profile. 

 

Also do you know how I include the canvases into my project files for sharing? I thought including them and saving would be enough, which I did. But clearly you had to import them seperately. In Blender you need to tick off an option to include the image into the file instead of using a local reference. But I didn't see this option anywhere in Fusion. 

Thanks again for the help!

Looking forward to your input

[TrippyLighting]

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@g-andresen wrote:

Hi Peter,

I have the canvas in the browser, but no content in the frame on the desktop.
Do you have any idea why this might be?

günther

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Nope! I've seen this only very rarely in other people's models, and I wonder if it has to do with the image format they use for the canvas. 

[davebYYPCU]

I wonder if it’s the grid - as I don’t use one, my canvases work ok.

I also have seen other supplied files with the problem.

Might help….

[TrippyLighting]

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@davebYYPCU wrote:

I wonder if it’s the grid - as I don’t use one, my canvases work ok.

I also have seen other supplied files with the problem.

Might help….

---

My grids are always turned off :

Yet, when I download the file I uploaded I see the canvas is lost in that file as well.

I'll have to investigate what format that is when I have time. There is another  canvas related bug I reported in detail 8 years ago (still hasn't been fixed!!!) that causes Fusion to mishandle the aspect ratio of imported images based on metadata.
I suspect this might also be related to image metadata.

[TrippyLighting]

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@Justine_makes_things wrote:

Hi @TrippyLighting Peter,

 What did you use for the curves?

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Five 3-point arcs. It took a little bit of patience adjusting the radii and the location of the points where they connect, but I suspect using a single fit-point spline is as much work.

I can create a screencast over the weekend to show the process as that isn't visible in a completed sketch.

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@Justine_makes_things wrote:

However, the sketch is still not fully defined? Do you know the reason for this? 

---

The reason is that Fusions code that determines whether or not s a sketch is fully defined still is far from bullet proof and gets it wrong in quite a few instances. This sketch is fully constrained, regardless whether Fusion likes it or not 😉

I am tagging @rohit.bapat to take a look at this sketch.

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@Justine_makes_things wrote:

I need it to be fully defined so I can make a new sketch on the extruded top side of the the profile. 

---

There are two reasons to fully define a sketch:

1. So parametric changes result in predictable changes in the sketch.

2. To avoid changes to a sketch by accidentally dragging a sketch object in the viewport when not actively editing a sketch though "edit sketch".

Fully defining sketches is good advice for new(er) users, however, if you are careful and considerate in creating sketches, the above can be achieved without fully defining a sketch. Not everything has to always be locked down. Just the "right things" have to be locked down. What "the right thing" will come with practice.

[Justine_makes_things]

Hi Peter,

---

@TrippyLighting wrote:

Five 3-point arcs. It took a little bit of patience adjusting the radii and the location of the points where they connect, but I suspect using a single fit-point spline is as much work.

I can create a screencast over the weekend to show the process as that isn't visible in a completed sketch.

If you find the time I would highly appreciate a screencast. I think learning with a project and help from fusion veterans like you will help me the most. Thank you.

About the un-bullet-proofness of the definedness:

That's unfortunate, but good to know! I'll try and cut out the the square on the top side without the sketch being defined. If I run into anymore problems I'll come back. I'll post the result when I'm finished. So maybe others can learn from this case too.

Update: I just finished the model. Thanks for the help!

[Justine_makes_things]

@TrippyLighting I found a way to get your sketch fully constrained. I added some construction lines and boom sketch fully defined. 

This youtube video helped: https://www.youtube.com/watch?v=23sS6y4KLpI

Unfortunately my sketch couldn't be fixed by drawing construction lines everywhere.

 

[TrippyLighting]

Nice video, but it's an unnecessary workaround.

I test my sketches exactly the same way. If I cannot drag things around, they are fully constrained. I have enough confidence in my sketches that I don't need that red lock.

Hopefully, @KristianLaholm reported that bug.

I don't blame him if he didn't 😉

Also, adding more "stuff," e.g., lines, doesn't always work. Here's a bug report @Phil.E 

[TrippyLighting]

@Justine_makes_things here's a screencast of how capturing the shape with arcs can be approached:

[Phil.E]

Thanks. I will send this to the sketch developers.

[sameer_babarNJS6C]

Hi,
As shown by @TrippyLighting in attached video, issue is reproducible from scratch.
Sketch seems fully constrained after initial analysis. We have created ticket FUS-156974 for further investigation.

Thanks,

Sameer Babar.


Autodesk Fusion Team.