How do I make 3d curves for sweeps?

[lukepighetti]

What are some good ways to go about making a 3d curve to do this type of sweep?

[NicolasXu]

Hi Luke,

I’m sure there would be various ways to build the 3D curves. For this model, we can probably leverage a 3D solid skeleton to build the curve. Please refer to the screenshot below for details:

Create a simple solid model.

Add necessary details.

The edge loop can be used for Sweep or solid Pipe or T-Spline Pipe commands. 

Or, we can start a new sketch and use ‘Include 3D Geometry’ command to copy the body edges as 3D curves.

Thanks,

[lukepighetti]

It looks like there is a function specifically for this called Intersection Curve

However, for some strange reason, you can only select one piece of geometry at a time. Strange.

https://screencast.autodesk.com/main/details/e1cc765c-bfc8-47d7-a75a-3c9e417ef874

[NicolasXu]

Hi Luke,

Thanks for bringing this out. The errors looks like an issue to me. I have asked the development team to look into it (ID: FUS-17019). As a workaround, we may extrude one curve loop as surface, and then use ‘Project To Surface’ command to generate the intersection.

Regarding the loop selection in Intersection Curve command, it's a current limitation & would be a good candidate of feature improvements. I have reported it to the development team for future consideration (FUS-17018).

Thanks again for your feedback!

[jjurban55]

I believe the reason you still need to select a plane for a 3d geometry, is it wants you to define which component coordinate system (CS) you want the geometry in (the active component CS will appear by default to select, but if so wanted to can make other component CS systems visible to select and hence be defined into).  

Jesse

[lukepighetti]

Except that it's 3d geometry. 😛 I cant think of a reason why someone would need to specify a plane when intersecting 3d geometry. 🙂

[kb9ydn]

Are there any plans to add 3D sketching to Fusion in the future?  I don't recall seeing it in the roadmap.

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[innovatenate]

@kb9ydn  There are some capabilities currently in Fusion 360 for 3D sketching, but make sure the option is enabled in the preferences. Check out the below screencast for clarification. I fumbled around for the option, but I found it hiding in the Design panel of preferences: 🙂

http://autode.sk/1Bp5F1Y

Is there something specific functionality you are looking for? I hope this helps. Let me know if you have any questions.

Thanks,

[kb9ydn]

---

@innovatenate wrote:

@kb9ydn  There are some capabilities currently in Fusion 360 for 3D sketching, but make sure the option is enabled in the preferences. Check out the below screencast for clarification. I fumbled around for the option, but I found it hiding in the Design panel of preferences: 🙂

http://autode.sk/1Bp5F1Y

Is there something specific functionality you are looking for? I hope this helps. Let me know if you have any questions.

Thanks,

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Oh ok; I see how it works now.  I was thinking of something like in Solidworks where you can press the tab key while sketching and it will change the active plane.  This video shows how it works (not me BTW).

https://youtu.be/HO-yg6sC5t4

Honestly I hadn't tried 3D sketching in Fusion until just now, and from the above posts it kind of sounded like you have to have existing geometry to reference for 3D sketching.  But after playing a bit I see that when sketching a line, if you drag the end point so that the line is parallel to the orthogonal axis of the plane you're working in, it will snap parallel to that axis.  Then you can tab between the angle and length to change them.  This is pretty cool now that I see how it works!

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[jjurban55]

Kb9ydn wrote: "...But after playing a bit I see that when sketching a line, if you drag the end point so that the line is parallel to the orthogonal axis of the plane you're working in, it will snap parallel to that axis.  Then you can tab between the angle and length to change them..."

I was trying to learn 3d geometry like this a little more, and can't quite make out what you were referring to, and would really appreciate a little clarification.  First, I tried moving a line endpoint off of its sketch plane using the move tool, but could not get it to snap parallel to the orthogonal coordinate system axis, except when out of the sketch and using the Align tool, which is pretty cool (is that what you were referring to?).  The thing I'm really wondering about, is what you mean by the "angle and length to change them", since to my knowledge you can't use the dimensioning tool on 3d lines, curves, points etc. (i.e. that have been moved off their sketch plane). 

Thanks for any help!

Jesse

[NicolasXu]

Hi,

Besides the ‘Project To Surface’ and ‘Intersection Curve’ command, there are several ways to create 3D sketches. Here is a screencast to show the steps.

• Align to X/Y/Z direction
• Use the Move command to move 2D sketch entities off the plane.
• Snap to objects while creating lines and splines (Not supporting the snap to sketch objects out of the active sketch at present. We have to use ‘Include 3D Geometry’ command as described below. It’s a known issue and the development team is working on it.)
• Use the Include 3D Geometries command. It can copy other existing objects (body edges, body vertices, sketch objects out of the active plane) into the active sketch and keep the association. We can then create more 3D sketch objects by snapping to them.

The idea behind why we need a sketch plane for 3D sketch, is that we wanted to someday deliver a unified 2D/3D sketch environment. You may refer to Jeff’s comments in the post below:

http://forums.autodesk.com/t5/general-fusion-360-questions/what-s-your-fusion-360-performance-like/t...   (post #53)

Regarding the dimension of 3D sketch, unfortunately, we have not yet been able to fully support it yet. What you both have observed is correct, i.e. after create 3D sketch line, you cannot use the dimensioning tool on the 3D sketch line; when you create 3D sketch line by aligning to X/Y/Z direction, you can input dimension like 2D sketch line. It’s probably an inconsistent case at present, but eventually we want to support both cases.

[jjurban55]

Thanks for that information Nicolas   Really powerful stuff.  And I never knew about that waiting while drawing a line to get that little coordinate system to appear, as I saw in that screencast.

Cool stuff.

Jesse

[kb9ydn]

Here's video that shows "tabbing" between the angle and length while sketching a line.

https://screencast.autodesk.com/Embed/Timeline/b794af1e-9d26-4c6b-bdff-b791ceecb353

If you move the mouse when doing this it gets kinda flaky.  I'm assuming they're still working on this.

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