Fusion 360 solids editing edges

[fabian.borg]

Hi,

I am new to Fusion 360 and would like to receive guidance to a problem I have. I need to have the ability to edit edges and or vertices of solids. I have seen tuts on getting this done by using forms, t-splines, etc. but somehow these are not getting the job done right. The model I am designing is a blocky type, (solid extracting from sketches) with cut holes and its full of right angles etc. hence when I convert from solids to t-spline (BRep to mesh), the model gets distorted badly.

All I would need is the direct ability to manipulate the edges of the solids and retain the shape but somehow I don't quite think its possible with Fusion 😞

Maybe I am missing something, hence please guide.

WBR Fab

[TrippyLighting]

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@Ajay_Kumar_Reddy wrote:

Of course you can do this using direct modelling(without forms)

1. Show the sketch in your design, hold the edges or vertices and try dragging them until you are satisfied with the output. the model will update as you move the edge or vertex.

you can perform the same operation using the forms.

2. Draw the profile and extrude it using forms.

close the profile using fill hole maintain creased edges. watch the video attached you'll get basic idea.

Hope this helps.

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What you are describing isn't direct modeling. You are still only modifying sketch entities and not actual model edges. that limits you to modifying only edges that directly coincide with sketch objects.

Your second suggestion using creasing I usually don't recommend because it creates NURBS surfaces. Even if those are perfectly flat, you won't be able to sketch on such faces. That is only one problem and you'll only get to experience that if the object even converts 😉

[chrisplyler]

Mesh modeling and CAD modeling are different things.

In CAD, you might approach such a shape thusly:

https://knowledge.autodesk.com/community/screencast/97e0452c-b774-4028-ba1f-1aac021ce902

[Ajay_Kumar_Reddy]

yeah, in that case you can't just edit any model directly even polymodels. Because you'll be modifying the underlying geometry in NURBS and in T-splines. press alt+2 to view the underlying geometry.

In this scenario our sketch is the under lying geometry. so we've just shown it and there's nothing wrong about it.

coming to creating the sketch on T-splines face, how could we create sketch on irregular face. we can create a separate plane by using the edges, offset plane etc., if the edges are straight and flat(faces).

[TrippyLighting]

You can directly edit edges of geometry of a T-Spline or Sub-D model. No sketches needed.

There are a number of reasons I don’t recommend modeling with creased edges in T-Splines.

A better method than creasing, although in simple models it often works, is actually to export the T-spline Control ca
ge, re-import it as a mesh and convert it directly into a BRep.

[Ajay_Kumar_Reddy]

you didn't get me.

I'm telling you that for direct modelling sketch is the under lying geometry.  we'll also be having the underlying geometry for T-splines(Edges and vertices for T-splines, for a sketch line and point. Name is different but the function is nearly same)

Generally we won't consider it for parametric modelling.

[TrippyLighting]

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@Ajay_Kumar_Reddy wrote:

you didn't get me.

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With more than 3 decades of professional experience in several CAD applications and 3D modeling in a variety of other modeling applications, that is possible but very unlikely.

Direct modeling does not involve changing sketch geometry. Period!

In Fusion 360 direct modeling does not involve a timeline, and as such changes to a sketch are NOT reflected in the 3D geometry originally created from that sketch.

The method you explained works (I suppose, I haven't actually tested it) bit is NOT direct modeling. Direct modeling works directly with 3D geometry, without sketches.

Here's some more advice. If you want to learn something, you'd be well-advised to listen to someone vastly more experienced than you. You provided advice to a user, which has consequences you were not aware of because you do not have enough experience.

[Ajay_Kumar_Reddy]

yeah, I agree and thank you so much.  You enlightened me.

[fabian.borg]

@TheCADWhisperer  I want to thank you for putting me on track, sketch modeling seems the ideal path for me. I wanted to ask you is how can I dimension a conic curve and make such defined (black) as I didn't mange to achieve that result as yet. The screenshot is a simple sketch of no particular reference, its just to demonstrate the blue line of the non dimension conic curve.

[TheCADWhisperer]

No *.f3d file Attached?

[fabian.borg]

@TheCADWhisperer  attached 🙂

[TheCADWhisperer]

In the Attached example I used two different dimensioning strategies depending on whether a Conic Curve was used or a Fit Point Spline.

There is no indication of your true Design Intent, so I don't know what you want to reference in your Conic Curve.

[chrisplyler]

A Conic Curve is defined by three points and a Rho value.

In your picture, you have snapped the first two points to the ends of fully constrained lines. Since when you do such a thing, Fusion automatically assume you want a Coincident constraint applied where you snap to something, those first two points become fully constrained by virtue of them being coincident to those line endpoints.

The third point (known as the Anchor point of the Conic Curve), however, was not snapped to, or otherwise made coincident, anything that is fully constrained, so it is not fully constrained either. That's why it's a white point in your picture. Since that anchor point is not fully constrained, neither is the curve itself. You could mouse-click-drag that white point all over the place without restraint, and the curve would move around appropriately.

You need to make that white Anchor point constrained. Either dimension it from the Origin point or some other constrained place, or use a Coincident or other constraint to definitively locate it AT the Origin point or some other constrained place.

[fabian.borg]

I would like to thank all of you for the help and support. I am sure to say that my first post here on the forum really enlightened me thanks to the great community here 🙂 Respect to all.

In particular I would like to thank @TheCADWhisperer for enlightening me to go for sketch based modelling of solids with dimensions, etc. Also I thank @chrisplyler for adding in further explanation that got me faster on track with the terminology of CAD.

Regards to all 🙂