Model is Disconnected - What does this mean?

[ptc-2192247]

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.

[JoseVidal]

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

[ptc-2192247]

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

[AnaFelizardo · Accepted solution]

Hello,

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

Title	Error “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!

[spete]

Ana-

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

[Natem0613]

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.