I have an existing assembly with a set of parts, one of these parts is a plate A which will serve as a support for a second group of parts which will also be placed on a plate B. To connect these 2 sets of parts I will have to make a support with 3 or 4 tubes of 10to 20mm bent in some places (a bit like chair legs).
Here are my questions:
1/ what method would be recommended to make the tubes, for now I wanted to make a sketch with a circle on a plane associated with my plate A, and a 2nd sketch that describes the trajectory of the tube, with the 2 ends coincident with, the center of the circle (plate A) and a plane created on the face of plate B on the other side. Then use the scan function to obtain a tube. In terms of sketching, I was just planning to do lines and sketch fillets for my elbows. Is there a better way to do it, which would take into account the reality in terms of possible bends depending on the material/diameter etc.? ?
2/ Since the existing assembly will, in the long run, contain 2 distinct sets of parts + the support that makes the link between the two, I guess it would be better if I took out the 2 sub-assemblies in separate assemblies?
3/ If so, can I design all my parts in the same assembly today, and later separate the whole thing into 3 assemblies (1 mother SDLASM that references the support + the 2 sub-assemblies)? What will happen to the sketch of my support (the one of the circle) since it will be linked to a plane that will have been created in relation to plate A (which is part of one of the 2 sub-assemblies).
4/ Will solidworks be able to help me determine the minimum diameter of the tube to be used according to the mass I want to place on plate B?
Agree with hdijoux, the welded construction is more practical since a single sketch is enough. If you don't have the tubes in your library, you can create them (sketch leab fit part) which you save in the weldment profile folder (C:).
Well it doesn't suit me too much, I have a support, and 2 sub-assemblies that contain my A and B plates, if tomorrow I don't want to solder the tubes anymore, but use plates/flanges screwed on the plates, I want to be able to do it.
It's not necessarily in the same part, you can constrain your two assemblies A and B in an assembly and add a mechanically welded part that binds to each of your assemblies.
Two solutions: either you use references in the context, i.e. your mechanically welded will need the assembly to be rebuilt because it will have its references in it. I only use this on small assemblies and only if the part can't be used for something else. The second solution is to create a skeleton, a 4th piece in your assembly in which you create a 3d sketch or plans or points, in any case something on which you can constrain your 3 sets. I use this when the assembly is too heavy to load in full, it allows you to open only a part (via configs) but to be sure of the positions.
For the 4th point, you have to pass your assembly in solidworks simulation, if you don't have a premium version of solidworks you can use the express simulation on the mechanically welded part. The express simulation assistant is quite simple, you enter the materials, so that it knows the mechanical property of matter, the fixed points (the points on the ground) and the external actions, gravities and forces applied on the part.
Put screenshots if you get stuck on something particular.