Make a Part's position same as its assembled position

[Drkwing]

I have 2 parts to be assembled.
- I add the parts to a product file and assemble them using Assembly Constraints(3d constraints)

- By using 3D Constraints, I reorient one of the parts with respect to the other. But this 'reorientation' is only happened in the product. When I open that part in its part file, I know that, its position and orientation is different from its assembled position and orientation.

-What I want is to set the part's original position and orientation to its assembled one. So that when I open the part in its part file separate from the assembly, I see that it rests in its assembled position wrt absolute cs.

How can I do this?

-Thus when I create a new product file, and add the parts by using 'add existing component', all the parts will fit in their correct assembled positions without the need for Assembly Constraints'.

Best regards

 

[Ashvanth]

Hi there..

1)You can apply the required orientation (translation and rotations) needed in the part level itself using the translate and rotate commands. This brings the part to its position in the assembly with the correct position.


2)alternatively you can create a WCS at the correctly position relative to the globlal (0,0,0) and start the modelling from there.

note:- these ways of creation of parts elinates the usage of constrints assy design.

 

[agumba]

the answer that you ask is the command that is at the assembly module in catia V5 called generate catpart from product. it is used for converting product to catpart.
its important property is to convert the product to catpart with locating at product so u don't have to move the data to original location.

 

[catiajim]

The biggest question is WHY? There are many answers to this question that can cause different answers to your problem.

If one of them is "because that's the way we've always done it", then I would argue that it's not necessary.

If your answer is "The OEM Requires it that way", then you will have to live with Create CATPart from Product if you can live with Isolated solids, or with Part Design Transform if you can live with the history of the transformations. But if you need to have the support geometry in it's assembled position, then the answer is "Start Over".

If your answer is "we need to have them in position when they are translated to another system), use the Create CATPart from Product, because the translation is going to isolate it anyway.