How to fully define sketches with splines?

[Anonymous]

So currently I am re-drawing this base (direct STL download or click here for an overview) for my GoPro Mount. I created the sketch that I want to extrude.

SketchI want  to keep dimensions as variable as possible so that I can change the angle (currently 25°) and the length of the top surface (longest line in the sketch). As you can see the lines are blue, so the sketch is not fully defined. Is it even possible to fully define the sketch with the two splines on the sides of this model?

As soon as I change the dimension of the longest line I get a skewed model and the form of both splines changes, which is not what I want.

SkewedKind regards

Maciej

[lichtzeichenanlage · Accepted solution]

Before I'm answering the question, I like to mention that you've two problems in your sketch. 

• You're using to many spline points. The rule you should have in mind is, using splines with the lowest possible number of spline points. This will not only result in better surfaces, it will also reduce problems in lofts etc. I've attached a version with less sketch points and almost the same look.
• You haven't included the origin (or other fixed and perhaps projected points) in your sketch - and this is already part of the answer. By not including the origin, you're not able to fully define the sketch and you'll allow sketch lines to flip around if you change dimensions in all directions

To fully define a spline, you have to dimension the handles, so that you can't move them anymore. You can achieve this by defining the length and defining the angle to other sketch lines. Constrains with other sketch lines are also possible. 

[Anonymous]

I don't get the part about including the origin in my sketch. How do I do this? And why exactly is this blocking me from defining a sketch fully? Is this just the way it works in Fusion 360?

[lichtzeichenanlage · Accepted solution]

• Normally you do this by starting a sketch path (line, circle etc.) at the origin. 
• In your sketch I've used two dimensions to fully define the sketch (I was low on time, moving might be an option, but often does not work out to good)

• The origin is a fixed point in the sketch and because of this nature you want to include it in the profile so the profile couldn't be moved anymore. By doing this, changes to the profile are (more) predictable. And this is called a fully defined sketch and they get flagged with a little pin.

[lichtzeichenanlage]

I missed to link a video about splines and surfaces:

[TrippyLighting]

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@Anonymous wrote:

I don't get the part about including the origin in my sketch. How do I do this? And why exactly is this blocking me from defining a sketch fully? Is this just the way it works in Fusion 360?

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Any sketch engine in any CAD software will require you to reference either the sketch origin, or projected geometry to fully define a sketch. At least Ive not come across one that does not in the last 30 years 😉

You need a solid immovable reference point, which is the purpose of the origin.

To include it you either start sketching at the origin, or - something I often do - you deliberately sketch away from the origin and then use a constraint to contain a sketch element to the origin.

[lichtzeichenanlage]

Yes, as usual @TrippyLighting description is more on point. I have to learn so much 😉

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@TrippyLighting wrote:

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... or - something I often do - you deliberately sketch away from the origin and then use a constraint to contain a sketch element to the origin.

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You mean drawing a line and using e.g. midpoint constrain? Yes, that's something I'm starting to to more often, too. You get center planes for free and that's often handy. Combined with symmetrical extrudes and you have two free center planes. 

[TrippyLighting]

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@lichtzeichenanlage wrote:

Yes, as usual @TrippyLighting description is more on point. I have to learn so much 😉

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@TrippyLighting wrote:

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... or - something I often do - you deliberately sketch away from the origin and then use a constraint to contain a sketch element to the origin.

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You mean drawing a line and using e.g. midpoint constrain? 

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Yep, exactly!

[mavigogun]

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@lichtzeichenanlage wrote:

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You mean drawing a line and using e.g. midpoint constrain? Yes, that's something I'm starting to to more often, too. You get center planes for free and that's often handy. Combined with symmetrical extrudes and you have two free center planes. 

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When you write "center planes for free", does this imply a symmetrical Sketch?   I'm all about free location of planes- if you can spare the time, an example that affords the referenced center planes would be much appreciated.

[lichtzeichenanlage]

Valid point. The plane would always be in the mid of the line but not always a center plane for the hole body. But I still find it useful in the stuff I'm doing (especially in combination with symmetrical extrudes). But you're right, it's not a "do it always" rule.

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@mavigogun wrote: 

When you write "center planes for free", does this imply a symmetrical Sketch?   I'm all about free location of planes- if you can spare the time, an example that affords the referenced center planes would be much appreciated.

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