Workflow guidance for designing pipe frame

[trevormead]

New to Fusion, coming over from Rhino and really struggling with some of the core principles and approaches. I'm trying to model a frame made from straight pieces of pipe and angled corner fittings. After watching and reading a smattering of tutorials and help articles, thought this would be the appropriate workflow:

1. Create a 3D sketch of half the frame, just as a placeholder for where components will be in relation to each other in space;
2. Model 3-way and 4-way fittings as separate components, use rigid joints to attach copies of each fitting to each frame sketch point, constrain fitting sketch lines to be parallel to frame sketch lines;
3. Extrude pipes from one fitting to the next and attach with joints, each pipe a separate component;
4. Mirror geometry to create other half of frame;
5. Model centerline fittings and pipe;
6. Parametrically adjust constrained frame sketch points as needed and watch Fusion magically adjust pipe lengths and fitting angles accordingly;
7. When finalized, export a list of cut lengths for all pipe components and 3D-print ready files of each fitting.

Based on the welts from smashing my forehead against the keyboard for several hours, I'm guessing the whole approach is wrong, or missing crucial steps. Could some kind soul help steer me in the right direction?

File attached, but for reference, here's a screenshot of the frame sketch, and an attached fitting down in the corner. The sketch for the fitting is just 3 lines, so ideally I'd want to align each of those lines to a line of the frame, so if (for example) I change the angle between two frame lines, the fitting sketch lines automatically update to match, if that makes sense.

[trevormead]

@TheCADWhisperer 

Ah, got it. File updated. Thanks again, can't tell you how valuable this walkthrough is!

[TheCADWhisperer]

@trevormead 

One more Split Face and then we will do a 3D Sketch for the remaining Pipe Paths..

Split these three faces with the YZ Plane

[TheCADWhisperer]

@trevormead 

Note the variable names for these two dimensions (yours might be different but on mine is d1 and d5).  You could rename these variables to something meaningful to you.

[TheCADWhisperer]

@trevormead 

Examine the Attached 3D Sketch file.

We could continue along this track, but I think it is easier and more robust to create 2D Sketches for these lines (and we wouldn't need the reference dimensions).

Then we can cut away excess solid geometry - or leave as is.

When/if we go to cut away - we will see "warped" faces.  Not sure you wanted warped or planar.

[trevormead]

I'd be curious to learn the 2D sketch alternative. Because the faces aren't planar (which is as expected), would it be four XZ sketches along each slice?

[davebYYPCU]

That’s what I was suggesting, No bottom sketch, it would be at the shoulder, but 6 of one and half dozen for the other.  

[trevormead]

Took a stab at the multiple 2D sketches, each sketch is created on the planes highlighted in the screenshot, fully constrained and tied to Projected points. Wasn't sure how to get the long straight lines running from front to back without a separate sketch ("Shoulder rails" in the file), wondering if there's a more efficient way to do that (maybe having the bottom sketch at the shoulder would solve?). Tried Projecting the points from the front sketch to each subsequent layer and couldn't get the lines to constrain.

@TheCADWhisperer 

 If I'm following, there's no need to trim the body to match the lines because the body will be irrelevant once the pipes and fittings are in place, so the body will be hidden while the pipe/fitting positions are adjusted via sketch edits; so we have the frame!

The original fittings were modeled after this approach from TrippyLighting some years ago. Inspired by our work here, tried drafting a proper constrained 2D sketch of the fitting and landed on this:

It's fully constrained, but the whole thing goes unconstrained when any of the circled constrains are removed, and I have no idea how translate this into a 3D object. Is this the right approach?

[davebYYPCU]

Removing constraints from a fully defined sketch = not fully defined.

Take all of the required profiles, left side of the vertical centre line.  Use the Revolve tool, and the Axis is that centre line.

Same for the bottom profiles of the horizontal Revolve, set join.

However, that sketch is unlikely what I would do to make the centre lines accord with the panel edges of the construction you are doing with the whisperer.  (Still not home yet)

Might help….

[TheCADWhisperer]

@trevormead 

Examine Sketch1 in the Attached.

If you are 3D printing rather than purchasing off-the-shelf, you can set the angles to whatever you want - not limited to 90° angles.

I would do these as individual files and externally reference into your assembly as needed and use Joints.

[trevormead]

@TheCADWhisperer 

Wow. That's much easier, amazing.

Reviewed the history and made edits to create a 4-way elbow with holes for a single button clip. Thanks for putting that together.

Hopefully the last question: since each of the sockets are defined via a Circular Pattern, is there a way to constrain each end to a line in the frame (something like a Collinear Constraint along the center point of each socket face)?

[TheCADWhisperer]

@trevormead 

Build your Pipes as Components.

Shorten the ends by necessary amount for the fittings. (Press/Pull, Offset or Extrude will do the job.)

Insert fitting and use Joints to assemble.

Learning Joints takes a bit but once you get the hang of it no big deal.

If you later edit and dimensions - the Joints (and location of your fittings) will automatically update.

[trevormead]

Alright, this is where I'm running into challenges.

• Created pipes as Components (highlighted curves or edges > Pipe > Grounded to Parent)
• Shortened ends to make room for fittings (Press/Pull > -1.50 in)
• Inserted 4-way elbow (Break Link > Ball Joint from orbit to frame point > some rotation for initial alignment)
• Lengthened first pipe (Extrude pipe face > To Object > face of small lip inside socket)
• Joined pipe to fitting (Rigid Joint between pipe face and inner lip face)
• Attempt to create Rigid Joint between another (non-aligned) socket and pipe and the joint fails.

Thought the Ball Joint might allow the elbow Component to rotate sockets as needed, and Breaking Link between the elbow Component and the parent file would allow it to morph as needed to fit the Joints.

How would I lock the pipes into place inside the fitting, but allow the fitting sockets to dynamically change angles to match the pipe positions? Almost feels like I'd need one sketch per socket, per fitting, with each sketch aligned to the target pipe plane (which also seems overly cumbersome).

[TheCADWhisperer]

@trevormead 

I haven't taken a look yet, but I would not use any Rigid Joints.

Mostly Revolution and Cylindrical Joints.

You cut too much off, should be 0.61

But is this going to align the pipes at these angles?

Are you going to 3D Print these connectors or are you going to use off-the-shelf connectors?

[trevormead]

3D printing the connectors, because they're going to end up being non-standard angles and configurations.

See what you mean about cutting too much off; length of each socket from the origin is 1.61, I want each pipe 1" deep, so only needed to extrude to the origin and cut .61. Roger.

Maybe I'm still misunderstanding the capabilities of joints; goal is to save time by having the connectors adjust simultaneously with the frame adjustments. So target workflow would be something like:

1. Fix connector origin points to frame intersection points via joints (so connectors move in space after a frame intersection point is moved)
2. Fix connector angles to always match angles between frame edge/curves (so connector ends automatically adjust their angles [in relation to the fixed origin point of the connector] after a frame intersection point is moved)
3. Extrude pipes from frame edges/curves, set pipe length as from "face of connector A" to "face of connector B" (so the pipe length automatically resizes after a frame intersection point is moved)

Is that possible? Or am I stuck editing the frame angles, then manually editing each connector to match, then importing each connector as-is and adjusting the pipes to fit?

[TheCADWhisperer]

@trevormead 

If the connectors are custom rather the off=the-shelf, then design in place so that they will update with changes in the frame.

[davebYYPCU]

Repetitive work, you will know exactly how it works by the time you get to the finished product.

Yes, the goal is to save time by having the connectors adjust simultaneously with the frame adjustments.  But you are over thinking it.  As I don’t know the extent of which parameters will be changing, I have done a demo of one Joiner, will come back after you review this process, so that any file dimension change will update correctly.

Your sketch 1.  My additional sketches. 

I made the first pipe Component with 2 ends and a pipe.

I have broken your sketch Planes, should be Offset origin plane to 1 point, not 3-point planes.

To build the Frame, add copies (New) of this Component to the pipe positions as required, with a Rigid Joint and using Midpoints as selected points.

Then I did the first Joiner - step the timeline and you will see what happens.

In summary, Make the Component (original is 17 inch). Move timeline to show the frame sketches and Loft bodies.

I moved Component 1 in the window and Capture Position.  Joint the Component to a pipe position of your choosing. (1st one)

In the Joint Dialogue set the angle for the clip hole to be facing as you wish, I have them all facing inside.

Decide on next position.  With Measure, measure the length of the new pipe, body edge or sketch line, click / copy to memory.

Next Copy Pipe component- Paste New (so important.)  You will get a new Component overlaying the original.

Delete the last Capture Position in the timeline, and the new one becomes independently visible.

Joint - rigid to midpoints - set hole direction.

Go to Modify > Change Parameters, Drill down to this new Component, and make visible Sketch 1 listing, Paste the measured value over the 17-inch entry.

Repeat until you have all the pipes done for a complete Joiner.

Modify > Combine > Join - select all the end bodies that are overlapping, then tick New Component - Untick this before selecting.  Do not keep tools.

You will find that all those bodies are joined to one body under a new Component (for Printing). Rename it.

Changing Parameters - 

(I have short cut this a fair bit for clarity - To do it correctly the centre line I am using, would have to be replaced with a projected pipe position article to position the end bodies, instead of this quick demo.)

The 14inch wide frame spacing, changed on its own will break my 3rd surface Loft, because the 4th vertical pipe will not be a straight loft. 

You will have to edit d13 because it is not 24 inches - your homework.

Might help....

[Ajay_Kumar_Reddy]

@TheCADWhisperer Amazing solution.

Made a IG Video explaining your method.