I have to design several wood boxes who will be bases for acrylic showcase boxes. They have all different sizes but the construction is the same and quite simple. So what I’m looking to do is to design a generic construction with constraints once, and then be able to change a few variables like the boards thickness, the thickness of the acrylic and the width height length of the box and I would get the dimensions of my wood boards to do the cutting.

I never used the assembly workbenches, can they be useful in my cases?

  • evasive_chimpanzee@lemmy.world
    4·
    13 days ago

    I did a very similar project. I was designing cabinet doors that all needed to look the same, but needed to be different widths. I did it before the update to 1.0 so the process is a little different now. I will say it wasn’t that hard, and I definitely parameterized way more stuff than I needed just cause I was playing around with it.

  • madnificent@lemmy.world
    3·
    13 days ago

    There is now a default assembly workbench. You don’t need it for this. It is mostly handy to verify your design.

    Assuming endless possible values: set up a spreadsheet, define an alias (top right) for the relevant values, and use that in your sketches and extrudes.

    You could model the various bodies in place in the right orientation and make do without any assembly as there are moving parts too. The new assembly workbench is nice to use though so it’s worth trying it out.

    • 1ko@lemmy.worldOP
      2·
      11 days ago

      Thanks. I just discovered the spreadsheet and aliases, pretty straightforward to use the values in the sketch. Now I have yet to find out how to create multiple parts.

      • madnificent@lemmy.world
        1·
        11 days ago

        That’s great!

        I’d create one body (the blue icon) per shape you want to cut. You can reference the same spreadsheet.

        If you want to reference geometry from another body, activate the body where you want to use it (doubleclick in the hierarchy), select the face of the other body, and use the subshape binder (the green icon with red dots I think). Calculating everything from the spreadsheet is the more stable option.

        Looking forward to see what you come up with if you choose to share it.

        • 1ko@lemmy.worldOP
          2·
          9 days ago

          Thanks, I created a first sketch+pad for the top plate on the XY plane, the the side plate on the XZ plane, now the side plate sit at the center of the top plate, how should I move it to the side of the top plate?

          • madnificent@lemmy.world
            1·
            8 days ago

            If you’ve made multiple bodies, you can place them by selecting the body in the tree view. Then open the scary property view, open the data tab, Base, Placement, Position.

            You can scroll to roughly put things in position but I’d use a formula in there so you can model in place and have a visual for each configuration.

            If you want to reuse a body for left/right you could make a clone or start thinking about the assembly workbench

            The data tab contains interesting info. Open it from time to time so it feels less scary. It allows to set the properties from a pad or update constraints from a sketch quickly. Moving a sketch around can be strange though as the axes are relative to the sketch’s coordinates.

              • madnificent@lemmy.world
                1·
                1 day ago

                Best I know of is TechDraw but that may not be as automated as you’d like. You essentially take the shapes and label the dimensions you want to show. Shapes/dimensions can be refreshed, likely also through a macro for multiple sheets if you need that.

                I don’t know the UI by memory but the flow is along the lines of: create TechDraw sheet; set scale; import shape; choose views of shape (top, front, …); add dimensions. This can be exported and printed.

                I think you can also save the current view of a sketch (save image or such in the menu?) but have not tried it and don’t know how repeatable that is and if you’ll run out of coloured ink in no time.

                Looking forward to look at your attached designs!

  • atomkarinca@lemmygrad.ml
    1·
    13 days ago

    if i understand this correctly, you don’t even need the assembly workbench for this because there are no moving parts. you just link your dimensions to cells in a spreadsheet from the the spreadsheet workbench and you’re good to go. (see the “Interaction between spreadsheets and the CAD model” section in the link)