Creating a line or sketch in 3D space (for a pipe sweep or channel sweep)

[Anonymous]

Maybe someone can understand what I am trying to achieve from these snapshots.

By the way it was very difficult for me to layout the circle sketch to the line shown above (its future path for its sweep).  I had to draw the circle sketch on a different plane and guestimate or eyeball a "move function" to align to the line in one plane and then do another guestimated or eyeballed "move function" to align in a different plane to ultimately achieve this layout.  Apparently the handy "align" function only works between components but not between sketches and lines even if a add a point to the endpoint of the line.

Is there a way two efficiently draw these types of structures?  I can't seem to find a practical way to have coincident lines drawn that jog at sharp 90 degree angles that create a pattern that is part of a 3D space rather than staying within a 2D plane.  Wish there were a way to attach the "triad" at the end point of the line and change the plane into which the line will extend like shown above.  This would allow someone to draw a line in 3D space rather than drawing segments and expend much efforts in trying to align components after creating them.

Maybe my challenge is that I am trying to use lines and construction lines and sweep paths to guide me in order to create a component, rather than making individual components and the stitching them together afterwards.  Sorry for my ignorance :-(.  HELP!!!!!  🙂  

Regards,

Emil

[Phil.E · Accepted solution]

Hi! Thanks for posting.

What you want is entirely possible. Construction geometry will get it done.

Steps:

1. Create your first sketch
2. Use Construct > Plane Along Path
3. Select the first sketch path
4. Drag the arrow to the end where you want another sketch to start
5. Okay the plane creation
6. Start a new sketch on this plane
7. Use Sketch > Project Geometry to project the end point from first sketch path onto this new sketch
8. Connect the second path to this point

This process can also be used to connect the sweep profile to these paths.

When you use Sweep you must select the paths in sequence.

Cheers!

[Anonymous]

Hi Phil,

Thanks you so much for such a quick and detailed reply!  See my version below...

Just one way to describe my current state, pure elation and joy.  THANKS AGAIN!

Regards,

Emil

[Anonymous]

Thanks for this

Took a little bit of time to understand the text instruction - the best way was just to plunge in and follow it - and it works - thank you

(A little screen cast my assist others in need)

Pulling the arrow seems to give it a value of 1 each time (so 0 being the start and 1 being the end point)

Shame you can't just type in the dimension like for everything else.

Anyway,  my question and request is - how can you apply a fillet radius to the 3D lines that are not on the same plane.

I had to make do with just filleting the corners of the extrusion, but in real life there would have been a full radius

eg 6mm round bar bent with 10mm radius corners - see enclosed screen shot

[Phil.E]

If you look at the dates, the original post was a couple years ago. Since then we have vastly improved the 3D sketching experience in Fusion 360.

Here is a short video showing a very basic workflow to create a sweep path in 3D, all in one sketch.

[jculleton3]

Ok. I understand how to draw a line in free space 3d but this is kicking my butt.

I am trying to connect two lines in two different planes that do not have a plane in common. 

Then I want to extrude a circle along the three lines.

Basically a u bent wire with the legs on opposite sides of a rotor or stator.

I have attached some images and I would like to figure this out without having to freehand the wires (they are specific length and positions.

I need to be able to do this several hundred times so I hope it isn't too difficult unless I can take the finished connected wire .070 inches in diameter and do a circular array?

[innovatenate]

Here's a Screencast showing one way you may accomplish this. It's a bit long-winded, but goes step by step:

I hope that helps!

[jculleton3]

Thank you for your quick response!

The only problem I am having is the locations are not 90 degrees apart.

I can convert both the lines to construction lines but when I edit sketch one disappears. Is that because I didn't project it into my other sketch?

In my previous cad program (all be it very limited) I could define each point in a line by X,Y,Z coordinates and just type the thing in.

I think the problem is the two points I want to connect are not 90 degrees in the Z direction.

The front line in inches goes x0.00 y1.89 z0.13 and extends down to x0.00 y0.50 z0.13. 

This line then crosses under and over at the same time to point x0.171 y0.47 z-0.65 and then traverses up and to the right x0.65 y1.785 z-0.65.

Does this make any sense?

I get the feeling from the screencast you did that I have to go 90 degrees in the z direction. This won't work for this drawing.

Thanks again and appreciate your patience with a newbie.

JC

I projected both construction lines (from two separate sketches) into 3D construction lines and I can draw the 3d line with all the angles.

Now I can't figure out how to do it into a circular array. No matter what I try it only selects some of the path not all of it.

[jculleton3]

Meh... I could draw it ok but now i am having problems with circular array...

[innovatenate]

Are you using the Create > Pattern > Circular or the Sketch > Circular Pattern command? 

I had some difficulty with the array the first time. I had to draw everything in one sketch and then dimension the overall angle between the two lines from the center point of the circular disk (not where they joint together on the inside of the disk). This angle let me determine the exact number of item and angular spacing of the circular pattern. 

I hope that helps. If it doesn't, perhaps you could record a short Autodesk Screencast to highlight where you are getting stuck?

Thanks,

[jculleton3]

here are three screencasts.

None of them accomplish what I want.

Maybe you can figure out what I am doing wrong from these.

[jculleton3]

screencast two

[jculleton3]

hopefully these help a little...

[innovatenate]

When creating the circular pattern, be mindful of the pattern type your are creating. I think you will want to create New Bodies and select Bodies in the Pattern Type:

I note that I created some additional path so that the bodies would align along the outer diameter once they've been patterned.

I'm not sure if that is necessary, but I thought I would mention it. It may help to upload and review the attached F3D file.

Let me know if this help or if you have further questions.

[jculleton3]

Thanks for the help.

I will look at it in about an hour.

No need to align the coils as they end up with crimp rings at the top. 

But the effort you put in is AWESOME!

Hopefully when I get to my machine I can replicate what you did with real values!!

The only thing that is still troubling me is the 90 connection thru the center. If I do a 90 across planes I have to use much room on the disc sides angling the wires over then up.

Thanks JC

[Anonymous]

I know your post is over half a year old, but I decided to see if I could recreate your shape to learn about 3D lines and splines. Here it is after I apply  a circular pattern:

One thing I wanted to mention -- you can set the xyz coordinates directly in the way you're used to from your prior CAD program. I made this by first sketching out the line segments in a 2D plane, just to create the points and roughly lay them out. Then I used the Move / Copy command to adjust each point. If you change the Move Type setting to "Point to Position," you can then input the coordinates directly.

[David_Ewen]

I'm attempting to run a 3D sketch + Line to do a sweep between 2 existing components. I can get 1 side to work but not the other.

As you can see in the photo, the left side where the 3D line and the circle sketch start doesn't and won't connect to the pipe.

The right side 

[Anonymous]

Thank you for this example! it was very helpful, I'm new using Fusion 360 and I was having trouble creating the skeleton for pipes.
That was an easy way to do it. But I have an issue trying to dimension the lines in a 3d space, the dimension command only works in the lines of the first plane.

Is it possible to re-dimension the lines of the 3d space once I've draw it?

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