Bridge curves for connecting pipes

[Anonymous]

I'm working on learning this software. I don't think Fusion has bridge curves where you can project lines on a pipe and then connect those lines with a simple bridge curve that is basically a 3d curve with an input you can use to dictate the amount of tangency curve you want?

In the uploaded file I had to apply a 'length dimension' to the spline curve to control the irregular shaped pipe. Now what I'd like to do is build some isoparametric curves on the surface of the pipe or just project lines onto the pipe so that I can build bridge curves which will be the guide curves for the loft command.  Is this possible in fusion?  I'd like full control of all these bridge curves I build as opposed to somehow building this shape in the sculpting area.

Thanks.

[Anonymous]

Can you edit an extruded sheet inside sculpt?  I extruded a pipe sketch I made in sculpt and for some crazy reason I can't lengthen the extrude distance, grrrrrrrr.

[TrippyLighting]

Look at lofting with rails. Unfortunately my screencast are not uploading at the moment.

Model is attached. Just walk through the timeline. I changed the tangent constraints in your sketches to smooth (G2).

[Anonymous]

Thanks, you helped me out a bit, BUT that spline curve you created is on a single plane.  I have uploaded a file for something I need to be able to produce.  I need to be able to generate a bridge curve b/w each fillet on the bottom piece to the corresponding line on the top cylinder so I can get a nice flowing look b/w the bottom square piece and top cylinder piece.  I need to create a bunch of these bridge curves/guide curves so I can slowly build the surface.   Is there any way to create a 3d spine to connect the bottom fillet curves to the curves on the cylinder in my model?

[Anonymous]

I think I figured it out a little, but I could use more help.....I just attached another model where I lofted the surfaces together....BUT is there a way to define the curvature other than just using the tangency option in the loft command?    I rather build all the guide curves then go around and build the surfaces....

It appears I can only adjust the tangency and that affects both the top and bottom connection tangency...I could use a little more flexibility, but I understand there could be limitations.  Thanks.

[TrippyLighting]

You mean like this ?

[laughingcreek]

I first saw @TrippyLighting drawing a 3d spline like this a while back, but he said in his last post his screen cast wasn't working, so I offer this.  Here is one way to do what you are asking. (I forgot to select g2 curvature on the loft in the screen cast.  that will improve the result)

[laughingcreek]

as we stumble over each other.

[TrippyLighting]

Yep, that's exactly how I created the spline!

When creating the loft I used the spline as a center line spline. It is counterintuitive that a spline that does not actually sit in the center can be used as a centerline spline but it works.

Also, when selecting the loft profiles in Patch mode I make sure to turn of the sketches so I select surface edges and not line segments or a profile in a sketch.

Then I also set the start / end. condition to G1 or G2.

That only works if the loft surface has something to be curvature continuous with and the cannot be a line segment, it must be a surface.

If the rounded edges on the rectangular profiles would be little spline segments with G2 tangency then the curvature of this thing would be even smoother.

[Anonymous]

Trippy/laughing....so many thanks, I may be in love with you right now lol.  I might be able to use this software 🙂  Thank you so much.  I am going to build out the model and see if it is what I am looking for.    Is curvature constraint basically just G2?

[Anonymous]

Trippy, what is the feature1 thing you are doing as the second to last step in each model, I cannot reverse engineer what that is or why?

[davebYYPCU]

Changes this

to this

helps stitch things together, with each part consistent. (Next step)  The two colours represent inside and outside in computer terms.

might help....

[Anonymous]

So I finished this learning project...here are my issues as discussed in this video:

1) Not sure if there is a better way to create a new plane in space at a specified point?

2) When projecting onto a surface, why do you have to select a plane? Doesn't make sense to me?

3) My first 4 lofts I did in my attached project do not allow me to choose a G1 for my 2nd profile

Thanks....here is my first video:

[davebYYPCU]

Well done sir, top marks all round, with a few tweaks to the workflows, you will enjoy Fusion.

I really like the video with questions explained. I may not be the guru but my thoughts might help.

1.  Yes would love an Offset plane through a point.  

If you know the length of the top construction line, then Offset the Origin plane and input that value, will be parametric.  Therefore no need to draw those llines.

2.  Offset to Surface, is also Create 3d Sketch, under the hood, All sketches in Fusion require a plane for its under the hood system.  Don't dwell on it.

3.  To get tangent conditions for the profiles, you need to hide the sketches and select the surface edges.  When you selected the demo profile, Fusion being Fusion did the fifty / fifty to show how clever it is.  I would not be surprised - maybe the actual outcome is as simple as the top is a curve and the bottom is a line, but edges is the correct way in my experience.

I think I have answered the questions. 

My 2 cents - can't replay the video while working in here - for the top section and 3d sketch routine - why?  

Surely you get the result, by extruding the circle, put a sketch on the bottom face for the square.

Can't remember, but looked like you lofted 8 times, and stitched, but Fusion can do one loft with two profiles and eight rails, might be easier, but I don't know the design intent.

Again a pleasure to get a video question.

[laughingcreek]

Just to address comment 2 one more time-

When ever you start a sketch command (such as line, or project to surface, etc.), if you don't already have a sketch active, then it FIRST runs the "start new sketch command", which requires a plane input for the sketch to anchor to.

But all that is moot in this case, because the command you needed there isn't a sketch.   Just go straight to"Split face."  works much better here to give you those edges.. 

[Anonymous]

dave,

thanks that fixed my loft error, I'm typically used to not clicking on lines but I guess I did somehow.

laughing,

thanks for the intel.  I attached a file with a simple project that is causing error.  I understand the split could be easier, but I'd like to find out why this is causing an error for me.

[laughingcreek]

Fails for me too when center axis line is used for the vector.  works when the construction plane is selected.  @jeff_strater, a bug?

[TrippyLighting]

@Anonymous A word of caution here. Never split a surface if it can be avoided. Splitting surfaces the safest way to have Fusion 360 or actually the ASM Kernel create crappy surfaces.

In this case the curvature is fine, but make sure to always check curvature with the curvature comb if you need to split a curved surface.

in this case you split the cylindrical surface with the open box to have edges too select for your splines to be tangent to. You could have just as easily split the open cube with the cylinder and have left the cylinder surface intact. 

[davebYYPCU]

I didn't think if Pete's answer with the box, 

but Alex didn't show you how to split the face, 

I deleted the offending lines in Sketch 3, 

modified sketch 2, 

created four 3 point planes, and split the faces with those four planes.

Clean but I like Pete's answer that fits your workflow.

Many ways to skin a cat.

[Anonymous]

Thanks, The split face is pretty easy, I'd actually probably intersect the plane onto the face of the cylinder. Of course that is a ton of planes and a ton of intersect commands.  I'd rather just project the square I built in the sketch, but maybe it's a bug as you said....it seems to be building out the lines, but causing an error.