open and closed positions of a part-best way to handle 1

[jaykm]

Hi all,
I have a small plastic wire grommet used to clamp the wires together. The legacy AutoCAD drawing shows the part in 'open' and 'closed' conditions (with diff. set of dimensions for each view- the part looks diff in each of the views). I need to make a new model & drawing for this.

Right now I am planning to create 2 part files (open,closed) and use "add model" option in the Drawing/detailing mode to create the drawing. Is there a better way of handling this?

Thanks in advance,
Jaya

 

[mloew]

jaykm,

I would suggest using Pro/PROGRAM functionality or a family table. Create the geometry that would allow for this toggle to happen. With control the configuration with Pro/PROGRAM, create a parameter that is called "clamp" (for example) and the value is "open" or "closed". Lets say that d47 controls the geometry that would move for it to be open or closed. Use this code in a relation:

if clamp == "open"
 d47 = 0
else
 d47 = 43
end

To do this with family tables, just create an instance for the closed or open version to have the same dimension modified accordingly.

To work with a print, the Family Table option will work better, but it is not as elegant as the Pro/PROGRAM relation way.

Good luck!

Best regards,

Matthew Ian Loew


Please see FAQ731-376 for tips on how to make the best use of Eng-Tips Fora.

 

[3dlogix]

I agree with Matthew, but this limits the part to only one state or the other no matter where it gets used.

Use Family Tables to create the open and closed parts. Thius way, you dont modify the same part throughout all assemblies by changing a single dimension.
In your drawing, you can add both model instances.

Steve

http://www.sprdesign.com

http://www.3dlogix.com

 

[jaykm]

Thanks matthew and 3dlogix for the feedback.
I could create a family table and could successfully create drawings out of the two instances.

As I am still learning pro/program in my spare time, this model may serve me well as a test example! :=). The tricky portion of the model is where one of the surfaces of the part that are flat when closed, become curved when open.I am not sure how do I handle this change from a flat surface (closed) to a curved surface(open state)

Thanks again for the feedback,
Jay

 

[3dlogix]

To handle the flat and curved surfaces, you can do a few things;

1- Make an actual flat surface and a curved surface that are independant of each other and have no children. Then select either one for the appropriate instance.

2- In your sketcher, try to make the flat surface using a very big radius value. The radius value would change as the instance changes.

Steve

http://www.sprdesign.com

http://www.3dlogix.com