"Magical" disappearing of an assembly component.

[ccruz]

Hello everyone!

This problem has been a pain for me. Apparently when you try to modify or reassemble a component that you inserted at the beginning of the assembly, the software "forgets" the most recent components.

I need to assemble an older component with a newer one and in order to do this, obviously I need both. Can someone please tell me how to fix this?

Regards,

Caonabo Cruz

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[AmitDeshpande]

Hi Caonabo,

The component definitely should not disappear like that.  It should be available for referencing when assembling the next component.

The issue could be related to graphics.  Could you try setting the config option graphics to win32_gdi and trying again?  Also, you could test on a different machine and with a simple assembly, just to see if the issue reproduces.

Please give this a try and let me know the results.  Also, upload the model here, if you would like me to test further with your assembly.

Thanks,

Amit

[Dale_Rosema]

Is the older part a family table? If so, it may be looking for a specific surface and when you switch to another instance, it cannot find that surface and therefor "drops" the part.

Thanks, Dale

[MartinHanak · Accepted solution]

Hi,

this is standard Creo feature. Imagine this assembly:

A1.asm

+ P1.prt

+ P2.prt

+ P3.prt

When you are editing definition (this means you are changing component assembling constraints) of P2.prt, then you do not see P3.prt because this component was not included in the assembly in time when P2.prt was added.

To see P3.prt you have to reorder components:

A1.asm

+ P1.prt

+ P3.prt

+ P2.prt

When you modify components (this means you are changing dimension values), then you can see all components.

MH

[ccruz]

Apparently, it worked... But I must ask you, how you knew this? I checked lots of forums and discussions and found nothing.

I mean, it's ridiculous how complex (complicated) Creo can be... The information of the software is so scattered and lets say, empirical.

Thanks Martin!

[AmitDeshpande]

Hi Caonabo,

This is actually the basic parent/child relationship theory within Pro/ENGINEER-Creo Parametric.

When in part mode, if you redefine a feature, then all the other features, listed below the feature being redefined, will not appear on the graphics screen, so as to maintain the parent/child relationship.

Same as in assembly mode, like Martin mentioned.  If you redefine the component placement, then all the components listed below it, will not appear on the graphics screen.

Thanks,

Amit

[MartinHanak]

Hi,

if you want to quickly learn Creo then pass certified Creo training course. I know it can be expensive ... But if you are self-learned then you are lost .

MH

[ccruz]

Amit and Martin,

Thank you for the support!

CC

[rohit_rajan]

Hi Martin how about using this config.pro option "comp_rollback_on_redef" ?