topic Re: modifying assembly in Fusion Design, Validate & Document Forum

modifying assembly

osh876 — Tue, 28 Sep 2021 12:43:26 GMT

i am making a frame with multiple vertical and horizontal parts, i have drawn each part of the frame as components as their own file, i then made a new drawing file where i can import all the parts to assemble them using the join command. i then join the imported components. but the problem i am trying to solve is when i make an adjustment of the length of a component in its original drawing, then update the file where the assembly takes place. but the length increase goes through the component joined to it, rather than the joined component moving with it.

i need away to make the drawing such that length modifications can be made and the component move accordingly

Re: modifying assembly

TheCADWhisperer — Tue, 28 Sep 2021 12:47:19 GMT

Can you File>Export your *.f3d (*.f3z) file to your local drive and then Attach it here to a Reply?

Re: modifying assembly

jeff_strater — Tue, 28 Sep 2021 13:19:24 GMT

Are you using "Joint" or "As-Built Joint" to create joints between your components? If you are using As-Built Joint, what you describe is expected behavior. That type of joint assumes that the two components are in the correct location, which is why you do not need to select geometry (faces, edges, etc) for this type. If you use just the basic Joint command, then the joint should react to component changes as you describe. But, in the end, that is all guesswork, unless you can share your design here, as @TheCADWhisperer said.

Re: modifying assembly

osh876 — Tue, 28 Sep 2021 13:33:23 GMT

i have attached a copy of a horizontal and vertical section, if you need anything else please let me know if you need anything else

Re: modifying assembly

TheCADWhisperer — Tue, 28 Sep 2021 13:43:50 GMT

I am a bit surprised that you would attach individual Components without the assembly file with the Joints that you used?

Also I notice that the profile sketches for your geometry are way too complicated, not fully defined and not making obvious use of symmetry about the Origin.

I would expect to have issues when not following robust techniques.

Re: modifying assembly

jeff_strater — Wed, 29 Sep 2021 01:03:56 GMT

there are probably many ways to do this. Extruded frame shapes like these are a challenge, because they tend to not have geometry in the places where you want to join them.

The video below shows how to approach this using some construction sketches and Joint Origins. I define some dimensions and a parameter for the width of the frame (though, as @TheCADWhisperer implies here, this sketch should be fully constrained for better behavior).

this width parameter is critical, because it allows me to position other joint origins on the sides of the frame piece, again using sketch construction geometry and that "width" parameter to position it correctly:

place joint origins at locations that are important to assembling these shapes. Then, once you have the Joint Origins placed, assembling is easy. Because the Joint Origins are associative to the geometry, and to that width parameter, they should update correctly when the length of the parts change.

I've included the modified design, FYI.