NX9 replace component "glitch" answer from GTAC 1

[animuL67]

This sounds ridiculous to me. Here is the issue:

"I have noticed one bug in NX 9 ever since we upgraded from 8.5. It is an issue in drafting where it does not allow you to replace a component that is in the drawing. This unfortunately leads to having to completely redo any view that is based off a component that changed, when normally it would be a couple of clicks and waiting 10 seconds for it to update.

The problem is outlined well in this forum post:

http://www.eng-tips.com/viewthread.cfm?qid=362010"

AND the response from GTAC:

"The problem where Replace component for drafting reference component not possible has been investigated and the following has been found.
Drafting Components are not real components and not part of the product structure; therefore, they should be treated as such for all practical purpose. They are special components intended to be used only by the drafting application to facilitate the creation of views of parts and were not designed to participate in the full offering of operations that standard Assembly Components do. Replace Component was not designed to support Drafting components and the execution thereof will lead to unwanted results and unintended consequences. The fact that Replace Component was allowed up until nx853 was due to an oversight and allowing it to remain in its current state will ultimately result in errors and poor quality for many customers.
That said, the decision was made to consider this for a future release. There are far too many issues with this functionality to simply re-enable as is. Proper analysis, design and testing are required in order to support these workflows if this is something we want to provide in the future.
"


So in other words: Sorry our software has been working so well for you, we fixed it so that you have a problem now. The thing is they say that it will results in errors but I have been using Unigraphics since version 18 ten years ago and have NEVER, not one time had an issue with swapping out a component like this.

 

[helperug]

NX_ENABLE_REPLACE_FOR_DRAFTING_COMPONENTS=1
give it try

sorry new in NX
regards
Erwin

 

[cowski]

Let's define terms so we are all on the same page...

A "drafting component" is NOT a real assembly component; it is simply a view that has been added from another .prt file. After adding a drafting component, no geometry shows up in the "modeling side", you cannot "assemble" it to the real components, and it will not show up in the parts list. It is only a view, not 3D geometry.

The option to use "drafting components" came about around NX 5. When adding a base view to the drawing, the default behavior (up until around NX 7.5) was to add a view from the current drawing file. This has changed in recent releases (a change for the worse, IMHO) to adding a view from a separate file. So while you may think you are adding a view of your model from the current drawing, you are probably adding a view of your model from the actual model file.

Drafting components do have their uses in certain cases; I believe they should be used as such - a "special case" command and NOT the default OOTB behavior! At least there is a customer default available to change the behavior (see thread561-375323).

So, while the "replace component" command has been working fine since at least v18 (and continues to work fine on actual assembly components), the option to replace a drafting component hasn't been around as long. The implications of replacing a drafting component were either overlooked at the time or not fully known until recently. I've been using UG/NX for about as long as you (v15); I can't think of many cases where functionality was removed in a later release. While I can't speak for Siemens, I feel fairly sure that the decision to remove it wasn't made lightly or without reason.

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