DV-What's New

Collaborative Modeling using Part Modules

Wouldn’t it be awesome if multiple designers could work on a single part in NX at the same time? Thanks to NX9 Part Modules this awesomeness just became a reality. Part Modules like it sounds allows you to build a part in a modular fashion. Different Portions of the same part can be worked on independently and those features can be merged together.
Below is a quick representation of how this process is achieved.

After a New Part has been created you have the option to start building within a part module right away or wait until you have the base model to a point in which you can assign it to a part module where it can be edited further.

For this example I’ll start with a simple Shelled block. Before I created any of the geometry I chose in the NX menu Format -> Part Modules -> New Module.

module1

I’ll name it Base and hit OK, Notice it appears in the Part Navigator.

module2

The green dot shows that this module is active and any design features I add will fall under this module.
Next a shelled block is created.

shelled

This is going to be the Base model in which other designers can work on. Before anyone can independently work on this part a module output must be defined. To do this select from the Menu Format -> Part Modules -> Define Module Output.
The output will be the entire body.

output1

Now that an output body has been specified any further editing to the body in this module will get published to this output.

A new part module must be created that can be made external so that other designers can work on it. You may want to make more than one depending on how many different designers need to work on this part at the same time. For this example 2 will be created.
Click the Green dot to deactivate the part module and create a new Part Module from the menu.
I will name this module Change1.
The new module should have appeared and is active. You’ll notice the geometry from the other module has been dulled out like it would be if you were in a different work part of an assembly. From here a Module Input needs to be defined, basically you are assigning how much of the geometry in a different module you will expose into this for another person to work on.
To do this go to Format -> Part Modules -> Define Module Input, Choose the new module as the Part module the geometry will be published to.

output2

Next select the geometry that will be published.

input1

Press OK and now this module contains a linked body of the previous module.

navigator

In order for this module to be worked on independently it needs to be linked as an external file. To do this go to Format -> Part Modules -> Create Linked Part.
Choose the module that will be made external.

external1

Click Ok and you will have the option to save the new Part
Once the Part has been created it is almost ready to be worked on by another person you must make sure that the linked part is closed to prevent file conflicts. Go to File -> Close -> Close Selected Parts
Make sure the part is closed by selecting it and closing it.

close1

Change.prt was the linked part I used. Once closed another designer can open the part and work on it.
In a different session of NX the file is opened by another designer, they will see the Part module that was created as well as the input body.

inputbody

Make sure the Module is activated by clicking the dot so it turns green. In this example some blends will be added to the shelled block.
Since this will be the only change that will be made in this module a module output should be defined with the body containing the changes.

blend

Before this module can be updated back in the original part file the module MUST be deactivated, clicking the green dot so it becomes clear will deactivate the module and unlock it. Now that the module is unlocked it can be saved and closed.
To pull in the new changes made to the external module, back in the original part file select Format -> Part Module -> Update Output References.
This will ask you to open the file up and update the linked module bodies. If a part was saved with the module still active NX will give a warning and will not update the part until the module has been deactivated.

deactivate

More modules can be created this way and linked externally, if a module is created using the previous module’s geometry the end result will be much easier to combine. For example Create a new Module using the new body from Change1 as shown above. Make it a linked external part.
Make sure both parts have been closed as shown before and make a change to the Change1 Module and a change to the New module that was created.

change2

In Change1 a Chamfer will be created on the top and bottom.

chamfer

The red square dots are a real-time indicator that these changes are new and that the module is not up to date. By deactivating this module the changes are automatically applied to the output body.

In Change2 Module a hole will be added in the center of the part.

hole

Deactivate and Save.
You’ll notice that when both module outputs have been updated , the chamfers still do not appear on the Change2 Module. To correct this you can merge the part module back into the main part file which will update all the inputs used. To do this go to Format -> Part Module -> Merge Module. Once both modules have been merged in the Changes will be applied to the final module in the List.

merge

And that’s it, you can make them external again after this and resave the parts or keep them in one file to send out. The new Part module feature really opens a new door for collaborative work that was much more difficult to do in the past.

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