How do you orient & combine multiple parts within a part file (NX5) ? 1

[RobLN]

I have a component which needs to be made from three other (different) existing parts - to save modelling.
So, I need to work out how to combine parts within a part file.

Within I-deas this would have been acheived by opening each part so that you've got the three parts on the work bench, orienting them to the correct position and then join. This would have created a 'bushy tree' with each joined element editable.

I have had go at this so far this is what I have tried:

1. Within the part modeler I open one of the three parts I need. Then File>import>part to grab the second one.
2. Then this dumps the history of the imported part chronologically into the existing history tree.

Problem is I can't seem to orient the imported part data to locate it where I want before I join it.

Please could someone let me know the best way to do this.

 

[uwam2ie]

try this:
open your assembly positioned as it is . Then file export part->dialog new - specify new file name - opject scope on all objects then class selection select all - > Ok new file is created - give it a try

 

[NXConsultants]

For future reference, knowing the NX version you are working with would be helpful.

Without seeing the part you're hoping to build these are a couple of suggestions based upon your question.

1. a. create a new part and add the 3 parts to it as components (making the new part in effect an assembly)

b. The move command can be used to manoeuvre the components in to the correct position/ orientation.

c. Use Wave geometry linker to add the body from each of the components, and then unite these solids in the new part. The part history for each part is held in each component.

2. Use the method you described (import) - Use Transform to move the solids around in the file - however you might have a few issues with parents of sketches not transforming as expected...

 

[RobLN]

Hi thanks for your response, I think thats a 'half solution' because once you've recreated the assembly as a new part there is no way to then edit the position of the pre-assembled parts that now make up the 'new part'

However, its helped me out thanks for giving me a start!

 

[RobLN]

Hi NXconsultants

Thanks for the pointers I'm using NX specifically 5.0.4.1

I've used the wave geometry feature for mirror parts before so I'll have a go at trying that for adding the bodies together as well.

 

[NXConsultants]

You could try assembly constraints - If you adjust the position of a component, the relative position of the linked body will update.

You've always got direct modelling.

Keep the unite feature as late as possible in the history so that you can move the feature ‘lumps’ around independently.

Ultimately the issue in the case is that NX and Ideas don't behave in the same way, relationships that are created in a separate part will maintained when that part is imported in to another, the history in NX is very sequential. The issue isn't insurmountable; it will just require an amount of rework.

I think you're going to like synchronous modelling...