More joint positions on one drawing

[Anonymous]

Hello,

I want to ask how can I create drawing of assembly with more different joint positions. For example imagine that you have assembly of folding knife and I want to create drawing with 2 views where on 1 view knife is folded and on second is open. As far as I know only one position is now possible for all views of one component/assembly. Or am I doing somethin wrong?

Thank you.

[jhackney1972]

Please excuse my crude model but you did not supply yours.  The process is pretty simple, just copy and paste new the blade component and show it in different joint position.  Create your drawing with two unique entries and suppress a component for each blade position.

[Anonymous]

Hello,

thank you for your feedback. This way I know but it is more like way around and if you have bigger assemblies with many joints it requires a lot of double work. So generally right now there is no function which would allow you to set different "positional representations" for assembly. Perfect would be if you set required values for your joints and then set it as representation A, then adjust joint values and save it as representation B. After that in drawing you could choose desired representation of component and you don’t need to care about coping and suppressing of parts.

[igelbriefkasten]

I am experiencing the same problem. The work around is ok, but with more than a handful of joints it can become a real problem. 

[Mublio]

This funcionality would be really helpful. We make cabinets and would like to show our customer both the interior and exterior of the design. This funcionality would allow that. 

[scottprater]

Old topic but easy solution for people still looking;

TLDR; use configurations to represent the open/closed position of your knife.

Longer explanation; Configurations allow you to suppress or unsuppress features in your design tree to create "configurations" of a model, say for example, with or without certain features.

With your knife model open and the joints fully defined, drag your knife to the closed position and select "Capture Position" (do this with the design history turned on; you should see the new captured position in the design history). Select the "Configure" tool, create a new configuration, click on the "Capture Position" in the design history, then select "Suppress." In your configurations table you should now see a "Positions" column next to each configuration. Clicking on the green check will turn it into a red dash and suppress the Capture Position for that configuration, returning the knife to the open position.

After you finish your configurations and save your model, now when you create a new base view, you have the ability to select which configuration you would like to show.

[Mublio]

Genius!