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ptc-21922471-Visitor
1-Visitor
July 20, 2009
Solved

Model is Disconnected - What does this mean?

  • July 20, 2009
  • 3 replies
  • 38603 views
Hello all, I did a search on this forum for an answer but have had no luck yet. I have an assembly open right now and in the bottom right of the screen (beside the filter) there is a blue "D" with a red "X" through it. Placing the mouse over this tell me that "The model is disconnected." What exactly does this mean? I have noticed this before, but i do not know if it pertains only to assemblies or not. Any help out there? Thanks in advance.
Best answer by AnaFelizardo

Hello,

I know this post is very old, but I found the following information on a PTC case.

TitleError “The Model is disconnected” when working with assembly in Pro/ENGINEER, Creo Elements/Pro and Creo Parametric.
Description
  • Error "The Model is disconnected" appeared when working with assembly.
  • Regeneration icon as changed to a crossed out D.
  • Regeneration manager replaced by a symbol of a D that has been X'ed over.
  • In the stop light for regeneration status, there is now a "D" with an "X" through it .
Applies To
  • Pro/ENGINEER all releases
  • Creo Elements/Pro 5.0 all datecodes
  • Creo Parametric 1.0 all datecodes, 2.0 all datecodes
Cause
  • One or more components are not fully constrained in the assembly.
  • Connections are not completed for some reason.
  • Assembly movement are running outside the limits defined at the connection
Resolution
  • Check / Redefine assembly component connections
  • Alternatives:
    • Set the configuration option enable_implied_joints as no
      • Warning message (x'D) will not appear in the regeneration display
      • Under constrained components will be treated as moveable (i.e. implied joints)
    • File > Prepare > Model Properties > Mechanism and change the Characteristic Length to a bigger value and then regenerate

Hope it helps anyone!

3 replies

J
JoseVidal1-Visitor
1-Visitor
July 21, 2009
Hi Scott, I had the same problem before and was unable to assemble any more parts. I don't know what it means but in my case I solved it by re-constraining a few parts that somehow got messed up. Don't know why it happened, never happened again and nobody seems to know what it means: neither in this forum, neither in MCADCentral, neither PTC Tech Support. I suggest you review your contraints and see if you find anything odd. If you - or anyone else - find out what this means, please share. Best regards! JVidal
P
ptc-21922471-VisitorAuthor
1-Visitor
July 22, 2009
Well i have tried to figure out the "D" with an "X" through it and I agree that it has to do with constraints. Most of the time, there is a traffic light in the bottom right corner of my screen and on assy's that are constrained correctly, this light is green. When a part is assembled and not perfectly constrained, it turns yellow, and then after that it turns to the dreaded "D". I dont know what causes this but maybe people are more familiar with the traffic lights and can explain those? Anyone? Regards
A
AnaFelizardo1-VisitorAnswer
1-Visitor
April 3, 2014

Hello,

I know this post is very old, but I found the following information on a PTC case.

TitleError “The Model is disconnected” when working with assembly in Pro/ENGINEER, Creo Elements/Pro and Creo Parametric.
Description
  • Error "The Model is disconnected" appeared when working with assembly.
  • Regeneration icon as changed to a crossed out D.
  • Regeneration manager replaced by a symbol of a D that has been X'ed over.
  • In the stop light for regeneration status, there is now a "D" with an "X" through it .
Applies To
  • Pro/ENGINEER all releases
  • Creo Elements/Pro 5.0 all datecodes
  • Creo Parametric 1.0 all datecodes, 2.0 all datecodes
Cause
  • One or more components are not fully constrained in the assembly.
  • Connections are not completed for some reason.
  • Assembly movement are running outside the limits defined at the connection
Resolution
  • Check / Redefine assembly component connections
  • Alternatives:
    • Set the configuration option enable_implied_joints as no
      • Warning message (x'D) will not appear in the regeneration display
      • Under constrained components will be treated as moveable (i.e. implied joints)
    • File > Prepare > Model Properties > Mechanism and change the Characteristic Length to a bigger value and then regenerate

Hope it helps anyone!

    S
    spete10-Marble
    10-Marble
    August 18, 2015

    Ana-

    Your post was the solution for my situation with a "Model is Disconnected" error.

    N
    Natem06131-Visitor
    1-Visitor
    April 7, 2020

    I had this problem with I had a few parts connected by a pin joints with both angles restricted. When I removed one of the angle restrictions and made the other parts not able to go perfectly vertical / horizontal my problem cleared up. I'm not 100% sure which thing fixed it, but there's a solution I had. 

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