3D note associative feature dimensions?

[amar.junankar]

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Hi,

When a standard hole is created in Pro/Engineer, a feature note is automatically created showing different parameters used. I am trying to do something similar for other features. E.g. displaying extrusion height in a 3D note attached to that extrusion feature?

This can be done by adding a parameter at part level, but can it be done by a parameter at feature level. If a parameter is defined in a feature and used in feature setup note, Pro/E doesn

 

[TonyJager]

Make sure you attach the note to the feature.


You should be able to insert the dim parameter into the note (&d0 for example). If that dimension is driven by a parameter insert the parameter into the note

 

[amar.junankar]

Hi Tony,

Thanks for your kind reply. I am able to insert dim parameter in note, but
not the parameter defined at feature level (even though note has same
feature as parent). I believe inserting dimension into note shold be sufficient
in most cases.

Thank you again,

Regards,
Amar Junankar

 

[TonyJager]

Amar


What you could do is the following. You can still show the parameter from the feature. You need to know the feature number and the parameter





ex.:


&TEST:FID_38 (TEST is the parameter and :fid_38 is feature number 38) you can get that from the feature info

 

[amar.junankar]

Hi Tony,

Thanks a lot!

I really appreciate your help. I was trying to get it work the same way
Pro/E does and then overlooked this FID use.

One similar problem I am struggling is to display a part parameter in a 3d
note in an assembly. I was trying to use session id for part (e.g.
&parameter_name:session_id) but it's not working.

Thank you again for your help.

Regards,
Amar

 

[TonyJager]

the proper syntax for this would be





&TEST:FID_39:4 (test is the parameter, :fid_39 is feature number and :4 is the feature id in the assembly)


Hope this helps

 

[amar.junankar]

Hi,

Thanks for reply.

If the parameter is not defined in any feature of part and is directly defined in Part file (e.g. Part_Name parameter), is there any method to display it's value in 3D note of an assembly?

Thank you,

Best Regards,
Amar

 

[rudresh.hm]

Hi tony,


I have one question on this.


can we control decilal places of dimension values used in parameters.


for example: I wolud like to creat a parameter for partdescription like : washer Dia 26 x 0.5 thick.


I want to show the dimensions of Dia and thickness wid two decilal places while the desciption parameter drive by these two dimensions should still show up the way I have mentioned.


thanks


-Rudresh

 

[sip]

Use parameter_name[.2] to limit the amount of digits shown to 2.


Sip
Edited by: sip