Solved: Control the value or state of a parameter value of...

danderson · ‎May 04, 2018

Hi,

Without using a layout, relations, pro-program or make flexible would there be a way to "Control the value or state of a parameter value of a part from a toplevel assembly"?

I want a part like a bolt to have 2 or more states built into the model that represents the bolt. Normal size as purchased (threads are full size and create a interference in the assembly) that would be used for the assembly drawing/weight roll up and a reduced size for FEA (part would not have interference with the hole it's installed into). The states of the component model would be controlled at the model level based on a parameter like "FEA" and relations to the dimensions of the features that need to be altered. If FEA was set to YES then the diameter would be reduced and if set to NO the diameter would be normal size.

At any higher level assembly I would like the ability without using relations, layouts, flexibility, pro-program or a custom toolkit program to be able to set all components with the parameter FEA to the value YES at any assembly level.

Anyone know of another way to do this within Creo Parametric/Simulate?

Thanks,

Don Anderson

pausob · ‎May 05, 2018

Sounds like you want to change the value of a parameter "FEA" in all parts that contain such parameter.

Here's one way to do it:

1) in your top level assembly, open the parameters editor

2) set the filter to "Current and all submodels"

3) sort by the "Name" field, scroll down to the rows with parameter "FEA". Then right-click on one of them and "Select all parameters with the same name":

4) Now they will all be highlighted. And now right-click again and "Edit Properties":

You can then change the value and it will affect all the selected rows.

Now after this regenerate the assembly and you should be good to go...

You can also set your own filter so that you don't have to hunt around for the "FEA" rows:

View solution in original post

pausob · ‎May 05, 2018