I have and assembly that I'd like to put on a drawing view. I want to show in an open and in closed state. Its a box with a hinge on it. Whats the best way to do this?
If you want to show it in the same drawing view.
Insert drawing view, then Insert-> Drawing view-> Alternate Position... From here you can select specific configarations if need for then hitting the green check mark. Then you will be taken back to your assembly model automaticly and the "Move component" command will be active. Move your door and hit the green check mark, and then you should see the 2 variant in your drawing view.
Hope that helps.
Joe if you want to show them in one view, then Lars's suggestion of Alternate Position View is the best to use.
If you looking to create two different views, then you can make two configurations in the assembly with closed and opened conditions. Then you can insert the views and change their properties.
In the drawing:
Lars and Deepak,
Thanks for the reply.
I currently have the assembly mated with coincident for the plane of the door and chest. I cant move any component when I ue Lars's method. When I use Deepaks method, do use derived config or regular config?
Also If i add another mate or ojbect to the assembly what' the best way to make the other configs have the same object and mate? For example, If want the chest to be 1 inch from the groung plane n both configs (open and closed) or I add a object in the chest?
Joseph, when you create an alternate position view, Solidworks adds a configuration to the assembly. So when it prompts you for the free drag, just hit OK. By suppressing or changing mates in that configuration, you can specify the mechanical variation.
Open your box assembly, active the alternate position confguration (It'll be called altpostion_default_1 or something similar). I suggest suppressing your coincident mate between the lid and box and adding an angular mate to show the open position. It's a good idea to do this so that you don't inadvertantly nudgee the lid and spawn drawing view updates.
Anyway, when you go back to your assembly, it should display both positions.
Joe check this if it helps: Alternate Position or Configuration in SolidWorks
I would probably use a derived configuration, assuming that you want everything except the postion of the lid to be the same between the two configurations. There is nothing sacred about that, just seems appropriate. Derived configurations can still be a little strange. I find it's best to check to make sure that the two configurations keep in step if I make a change to one of them.
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