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NX12 Assemblies - Drag and drop behavior

Siemens Phenom Siemens Phenom
Siemens Phenom

NX 11.0.2.7 MP6

With an open assembly if I drag and drop a part from OS to NX GUI (native) , it pop ups 'Assembly Constraints' dialog. Can create constraints and the part gets added to the assembly as a component. Now if I again drag and drop another part in GUI and hit cancel on the assembly constraints dialog, it does not add part in the current assembly. As expected.

 

NX 12.0.0.27 MP3

Now in NX12, for drag and drop method if cancel action is performed on assembly constraints dialog, part gets added to the assembly as a component without constraints. Smiley Surprised

 

I know there are enhancements to the add component dialog in NX12. As in both the versions, drag and drop method pop ups the assembly constraints dialog. So, irrespective of enhancements, the behavior should be the same in both versions.

 

Probably a bug?

14 REPLIES

Re: NX12 Assemblies - Drag and drop behavior

Valued Contributor
Valued Contributor

In NX11.0.0.33 if you drag and drop a part and hit OK it will add the part without constraints.

If you hit cancel, part is not added.

 

I agree it should be consistent between versions.

Re: NX12 Assemblies - Drag and drop behavior

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

now if it's will add the part without constraining in a higher version it can be an enhancement.

If it's not possible in a higher version then it's not consistent or there has to be a good explanation why it's not there any more.


Ruud van den Brand
Pre-sales NX CAD
cards PLM Solutions

Re: NX12 Assemblies - Drag and drop behavior

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

I rarely use the drag & drop method, but I can see the logic of this being an intentional change. When you drag & drop, your intention is to add the part to the assembly. Why would cancelling the constraints dialog abort the entire add component operation? If I create a block in a part then start the "move object" command but change my mind and press cancel, I don't expect the block to be deleted.

 

Take the above with the proverbial grain of salt. I don't know if this is the actual reasoning behind the change or even if the change was intentional.

Re: NX12 Assemblies - Drag and drop behavior

Siemens Phenom Siemens Phenom
Siemens Phenom

Also, a big change in 12 is, apart from the drag and drop. In 11.0 you could add the component, got the select/add component menu, and after that you are in the position/constraint menu. In 12.0 the add component and positioning menu have been combined. I believe the base of the changed behavior lies in this. But would be good to know this was an intentional change or not.

 

Maybe @TaylorAnderson could shed a light on this?

 

Kind regards,


Dennis

Dennis de Brouwer
Application Support Engineer
GTAC EMEA - Siemens Industry Software

Re: NX12 Assemblies - Drag and drop behavior

Siemens Phenom Siemens Phenom
Siemens Phenom

Dennis --

 

I'm flattered that you thought of me, but I don't know this specific answer.  :-)

 

But I will contact my Assemblies counterpart and see if he can help with the details.

 

Thanks!

Taylor Anderson
NX Product Manager, Knowledge Reuse and NX Design
Tel: +1 (602) 441-0683
taylor.anderson@siemens.com

Re: NX12 Assemblies - Drag and drop behavior

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi Ganesh,

 

This behaves as may be expected.

Previously the UI was of the old type where there were "many sequential dialogs in a command chain". Maybe you remember that even extrude used to be like that?

This type of UI has been abandoned. In the current standard UI a command usually uses a single dialog with the occasional spawned dialog . From a spawned dialog you always get back to the main dialog for pressing OK or APPLY to complete the command.

 

The cancel behavior for the old and new is different. In the old UI pressing cancel, cancels the stack of dialogs. In the new UI drag and drop is considered its own command. We allowed assemblies constraints to start because we are all used to that happening. But assembly constraints is its own command. 

 

To go back to the state before drag and drop: cancel the constraints dialog and press undo to undo the drag and drop.

 

Regards, **bleep**

 

 

Re: NX12 Assemblies - Drag and drop behavior

Siemens Phenom Siemens Phenom
Siemens Phenom

Thank you all for your valuable comments! Smiley Happy

Re: NX12 Assemblies - Drag and drop behavior

Valued Contributor
Valued Contributor

Hi  Dic k,

 

from monday 18.6. i started using NX12. I am little bit disgruntled, because i was plenty using drag&drop(in NX8-11) for add of components from OS to Assembly. Now with new UI it put me to way still setting of "Assembly Location" as "Snap". I hope is there some default setting, where it is possible to set on other choices. My favorit is "Absolute - Displayed Part".

 

Please, be so kind and tell me, where can i set it.

 

Regards, GL

 

Re: NX12 Assemblies - Drag and drop behavior

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi,

 

You can still set the default behavior to ABS origin in the customer defaults as before.

Go to customer defaults --> Assemblies --> general --> component operations tab. Then set single select drag & drop to skip the add component dialog and position to absolute origin.

 

I hope this works for you.

 

Regards, **bleep**