Relations Creo 11 Bounding Box to Parameters

[DC_9850851]

Hello, I am trying to create a map key that will auto create the new "enclosure volume" feature then take its x,y,z dimensions and add them to a parameter in my bill of materials. My biggest issue is the enclosure volumes parameters have an "internal feature ID" attached to them and is unique between components if I want to reuse this map key which then causes failures in the relations for PTC_BBOX_X:FID_(should have an ID number instead of stars.) I tried to incorperate copy and pasting the the feature ID from the feature information but that part of the map key doesnt work as it only pastes what was copied when map key was made. I also tried inserting the bounding box parameters in the map key and that failed as well because it cant find the parameters agian because of the internal feature ID.

Here are my current Parameters:

FINISH_SIZE string

XR real number

YR real number

ZR real number

X string

Y string

Z string

Here are my relations:

XR=CEIL(PTC_BBOX_X:FID_****,3)
YR=CEIL(PTC_BBOX_Y:FID_****,3)
ZR=CEIL(PTC_BBOX_Z:FID_****,3)
X=RTOS(XR)
Y=RTOS(YR)
Z=RTOS(ZR)
FINISHSIZE=X+"x"+Y+"x"+Z

The XR, YR, ZR relations are to take the values of the bounding box parameters and limit them to a rounded up 3 decimal real number. the X, Y , Z rtos relations are to convert the real number to text string. The finish size relation is to tie all the text strings together from X, Y, Z strings to make the size of the block for a BOM. example 5.1x.155x2.51. 

Any solutions to what I am trying to do?

[tbraxton]

I have not verified this yet (not running Creo 11 yet), but you should be able to use the mapkey in part mode for each part. This will create feature parameters in the part enclosure volume feature. This will take care of the mapkey re-use issue. Apply the relations to the feature parameters in the parts to round off the values and convert to string etc.

Create a BOM table with repeat region that will call the derived string params for x,y,z of each part. 

[DC_9850851]

Thanks for the response I failed to mention this was all in the part level already.

[tbraxton]

The mapkey works in part mode for all models? All features in Creo have a unique feature ID. I am not sure why you are having to include the FID in relations in the part where the relations are defined. I think I am assuming or missing something with your workflow. You can also use the feature name in lieu of the feature ID if I recall accurately. You can then standardize the feature names for the box params and the mapkey would work on all models with the named features.

[tbraxton · Accepted solution]

Here is how to substitute the feature name for the ID. This assumes you have user defined feature name where required to support the relations definition.

If you write a relation in the feature’s parent model (part or assembly) or in another feature, you must use one of the following formats to reference that feature:

XYZ = parameter_name:fid_N

or

XYZ = parameter_name:fid_feature_name

[DC_9850851]

Thank you for the help!

By changing the name of the feature in the model tree it automatically removed the FID #s and replaced them with the feature name.

XR=CEIL(PTC_BBOX_X:FID_8785,3)

I didnt quite understand what you meant until this happened.

The FID_8785 changed to FID_BOUND  when I renamed the Volume Enclosure feature name to Bound.

XR=CEIL(PTC_BBOX_X:FID_BOUND,3)