Steel square tubing framework from complex sketch

[ecorm]

you will notice that for the angular tube, the thickness function does not work, I had to make a full and a hole and subtraction

I'm trying to do the same as you, but I'm stuck. I'm trying to create individual sketches for each tube segment using my main sketch as the master sketch, using the technique shown in https://www.youtube.com/watch?v=2Yee1pSqTLg

When I attempt to use the External Geometry tool (https://wiki.freecadweb.org/Sketcher_External) to copy vertices from the master sketch, I get "Selecton not allowed by filter" in the status bar, followed by "Not allowed: CellFrame.Model.Body.Sketch".

Here is a screenshot of my model tree:

ModelTree.png (17.45 KiB) Viewed 2018 times

where:

• Model is the Assembly 4 model
  Sketch is the master sketch as shown in my original post
  Sketch001 is a sketch intended to capture a tube segment
  Master contains a master spreadsheet used by all my subassemblies

[papyblaise]

you can not use the exterior refs from one body to another
only the sketch workbench allows it outside of Partdesign
these are the limits of Partdesign

[ecorm]

I ended up resolving my External Geometry problems by moving the master sketch outside of the Body under Model, then using ShapeBinder.

I was then able to generate a solid segment via Pad, then hollow it out via Thickness.

FrameSegment.png (32.57 KiB) Viewed 1995 times

The end towards +Y wasn't cut open properly, presumably because that edge in the sketch wasn't square with the tube's sides. I can make it square and then use the appropriate cutting tool.

I realise now that Sweep would allow me to more accurately model the curvature of the steel tubing corners. Not sure if it'll make much of a difference in the volume/weight calculations.

I think I can figure out the rest from here. Many thanks for the help!

[ecorm]

I redid my master sketch with only the right half of the drawing, with the intent of using mirror operations. I also removed some duplicated explicit length constraints, using the equal length constraint where possible. It's much cleaner now.

OverhauledSketch.png (73.6 KiB) Viewed 1953 times

I also figured out how to make one continuous pipe out of two segments where it should be completely hollow without any internal walls once welded.

CellFrameTwoSegments.png (38.41 KiB) Viewed 1953 times

The steps were:

1. Place the MasterSketch under Model so that it can be referenced by multiple bodies in the assembly (there will be four pipe bodies).
2. Create a ShapeBinder with the edges needed for the continuous pipe, selected from the MasterSketch.
3. PartDesign.Pad the ShapeBinder to create a solid.
4. (Not shown) PartDesign.Mirror the solid
5. PartDesign.Filet the solid's long edges to model the corner radius of steel square tubing.
6. Select two faces at the ends of the solid, then apply the PartDesign.Thickness tool with inwards thickness in Pipe mode.

The order of those last two operations is important if you want to filet both the outside and inside of the tube.

I had also tried to Sweep a sketch of the pipe profile along the path of the pipe, but I gave up due to the difficulty. The way I did it as described above seemed such easier.

I hope this helps someone else trying to do something similar.

P.S. That 45 degree corner brace doesn't seem to do much structurally, but it's actually there to mount a whiffle tree that will support the mirror when tilted (not shown).

[chrisb]

Would you mind uploading the file?

[paullee]

Maybe you can try the Dodo Workbench (previously Flamingo) which is very handy to produce steel structure.

[ecorm]

Maybe you can try the Dodo Workbench (previously Flamingo) which is very handy to produce steel structure.

I tried that, but it complained about there not being a Draft. I have to base everything off of a Sketch due to the necessity (and desirability) to use constraints.

[ecorm]

Would you mind uploading the file?

Sorry, but I'm not willing to share this with the world at this point. I know I might not be following best practices, but this is just for a hobby project.

I'm not stuck anymore, and I appreciate all the help everyone has given me here.

[chrisb]

Sorry, but I'm not willing to share this with the world at this point. I know I might not be following best practices, but this is just for a hobby project.

That's rather uncommon, especially because it is a hobby project, and others could learn from it; but of course it is your decision. Is there a certain design goal behind the complicated sketch with all its triangles? Are there given design parameters?

[ecorm]

Is there a certain design goal behind the complicated sketch with all its triangles? Are there given design parameters?

See the product photo in my original post concerning what the triangles are. They are what hold the support points that make contact with the telescope mirror. The triangles pivot on a spherical bearing, and the bars that hold the triangles can also pivot. The overall design is what's called an "18 point mirror cell" and is standard practice for telescopes of the size I'm planning to build. The design parameters for the triangles come from specialized software called PLOP. It calculates the optimal placement of the mirror support points, as well as the triangle's pivot point, in order to minimize the deformation of the mirror under its own weight (at the sub-micron scale).

The positions of triangle's pivot points determine the placement of three of the frame pipes. Thus why there were so many triangles in my sketch. However, it turns out I didn't really need the triangles within the sketch of the support frame. The triangles are now in a separate sketch within what I call a "triangle plate" assembly.

There was another reason for all the triangles in the sketch, having to do with me with me wanting them equilateral, but PLOP doesn't generate equilateral triangles. I was relying on the sketch to make them equilateral. I've since changed my mind; they are no longer equilateral. You can read all the gory details about this here if you care to: https://www.cloudynights.com/topic/7688 ... oint-cell/

I've since learned that calculating a bit of geometry within FreeCAD spreadsheets can remove a lot of construction lines in the sketch.

Here's my current simplified sketch without the triangles.

SimplifiedSketch.png (56.25 KiB) Viewed 1835 times

My (incomplete) mirror support with the triangle sub-assemblies is coming along nicely, IMHO.

MirrorSupport.png (65.15 KiB) Viewed 1835 times

If my telescope turns out to be successful, I might change my mind about sharing the CAD file. For now, I don't want to be blamed if others use this unproven design and it fails on them.