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Additional Component when Added into a Drawing

Pioneer
Pioneer

I have noticed that when I include a view of an assembly component into a drawing for the top level assembly, NX is adding another component to my assembly.  So basically, if I have an assembly -010 and there are two -010-001 components that are part of that assembly, if I add a view of the sub component -010-001 in my drawing for the -010 top level assembly, NX adds an additional -010-001 to my -010 assembly, so no my tree says that I am using three -010-001 components instead of the two that are actually part of the assembly.

 

Additionally, if I export the -010 top level assembly, I end up with an extra -010-001 in a completely different coordinate system.  We've worked around the problem in the past, but I'm sure there is something that I must be doing incorrectly or a box I'm forgetting to check that is causing this issue.

 

Any assistance would be greatly appreciated.

 

Thanks

 

4 REPLIES

Re: Additional Component when Added into a Drawing

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Have a look in the customer defaults and try turning off 'Create Drafting Component' (see image below).

 

2017-01-25_15-56-45.jpg

 

 

 

 

Anthony Galante, Senior Support Engineer
PhoenxPLM
24 versions of NX installed: NX4 to NX12, plus TC11.2

Re: Additional Component when Added into a Drawing

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Ignore my last response, it won't fix your problem. There's an ER about this:

 

  • How to don't make "reference component" in drafting?
  • Symptom
  •           PR Number:	2208502
    	   Priority:	2
           GTAC Urgency:	No
    	  PR Matrix:	6b
        ============================
    
    Problem Description: This case reports the problem where "Unable to avoid reference component in drafting".
    
    =============================================================================
     NX Versions:	NX 8.0.2
    Managed Mode:	No
     Tc Versions:	n/a 
    
    Containing:
    -----------
    Part:		n/a
    AVI:		comp.avi
    Syslog:		n/a
    Other Files:	n/a
    
    Steps to Duplicate: 
    
    1. Make assembly below.
        Assy
          COMP1
          COMP2
    2. To make solid body in COMP1 or 2
    3. [Start] - [Application] - [Drafting]
    4. To make sheet to Assy
    5. [Insert]-[View]-[Base...]
    6.„@To select "Part" in Dialogue box.
    7.  Select Part - COMP1 or 2
    8. Made reference component.
    
    Please refer the AVI for more information.
    
    Workarround
     Use Advanced Weight Management-Assert Values.
         Set reference component mass is 0.
    
    Problem is part specific:	No
    Problem is OS specific:		Unknown
    
    Platform Information-
    Problem is platform specific:	Unknown  
    
    Problem verified on the following platforms and OS versions:
    NX Versions Reproduced In GTAC: NX8.0.3.r, NX8.5
    OS Versions used during Test: Intel Win 7 64Bit.
  • Solution
  • The problem of avoiding "reference component" in drafting has been investigated and the following has been found.
    We currently do not support creating drawings of "view of part" without creating a drawing reference component. The setting "Create Drafting Component for view of Master Model Part" is a special case for master model only. So, I am converting this into an ER.
    Regarding the assembly weight calculation, there is a customer default "Exclude Reference Only Components from Weight Calculation" under Analysis->Weight Management to exclude such components from the weight calculation.
Anthony Galante, Senior Support Engineer
PhoenxPLM
24 versions of NX installed: NX4 to NX12, plus TC11.2

Re: Additional Component when Added into a Drawing

Pioneer
Pioneer

Thanks for the feedback - seems like a pretty standard practice that should be supported.

Re: Additional Component when Added into a Drawing

Valued Contributor
Valued Contributor

You can hide reference only components in the ANT by unchecking "include reference only components."  What are you using to export your structure?

 

Never heard of what you're trying to do - if you're adding a view from a part that's already in your assembly then your structure involves drawings which tree into other drawings, this is completely contrary to modern master modeling techniques.