I want to make a detailed plan of a manhole, not drawn as a sub-assembly, with all its components (ferrule, reinforcements, flanges, bolts, joints...) while keeping the link with the original assembly. It would be very appreciable if the reference numbers of the nomenclature of the detailed plan corresponded with those of the overall plan.
If this is not possible, how can we convert parts inserted into an assembly into sub-assembly? This way I will be able to make a drawing of this sub-assembly (at the risk of not having the same reference numbers as the overall plan).
To create a subassembly, you can select your parts and right-click form a subassembly. Solidworks will ask you to save your subassembly and create it in your assembly. Beware of the constraints that may have to be repaired.
Otherwise, to keep your bearings, you can create a configuration in your assembly where you leave displayed (you delete the others) only the components you want and use this configuration for your drawing.
Or, you can hide the components you don't want to display on a drawing view (click on the component and show/show the component).
In view of the request, I think that @dargaud.anthony's 2nd solution is the easiest.
You make a configuration in the assembly by "removing" all the parts that don't interest you. Then you insert a new view by selecting this drawing (right click on the view, property, choice of configuration)
On the other hand, be careful, if you insert in a new sheet, remember to right-click on your view => property => "bubbles", link to the other N°XX (where the XX is the N° of the nomenclature of the 1st sheet). Just to have the same bearings;)
Hello, (I see that I was too long to write my answer...)
You have several solutions:
- Create a configuration in your assembly showing only the parts concerned by this drawing and then draw the assembly in this configuration
- Make a drawing of your assembly and then hide the parts not concerned by this drawing in the design tree of each view (it's tedious and DIY but sometimes there is no choice)
- Make a sub-assembly (In the design tree of your assembly, select the parts concerned then right-click and "Form a new subassembly". Then make a drawing of this assembly.
To keep the numbering of the general assembly, you can create several boards in your drawing, in one you put the general assembly with the nomenclature and in the other the sub-assembly (it also works if everything is on the same board). You right-click on the subset view and in properties: "Link the balloon text to the specified table": select the nomenclature of your first spread.
Another solution: create a custom property in your parts which will be the reference number of your part and then you create a bill of materials using this property as the article number. Advantage => allows you to have a bill of materials by subset. (with a tite macro to fill this property)