Patterning a pattern in Pro/ENGINEER

'Pro/ENGINEER Tip For Patterning A Pattern'
Most newer, and several experienced, Pro/ENGINEER users are of the belief
that you cannot pattern an existing pattern of features. This is not
necessarily true. There are ways to do this--so that the user can leverage
existing patterns of features to speed up the model creation process with
regards to feature duplication. Below you will find a couple of different
ways to pattern an existing pattern of features in Pro/ENGINEER:
1) Create a datum axis using the #Two Planes option--making sure to
dimensionally locate it with respect to a couple of stable references by
utilizing the #Make Datum; #Offset functionality for both datum planes.
NOTE: You can replace the first datum axis with an #On Surface datum point
that is located with respect to two surfaces and achieve the same results.
2) Create your feature to be patterned, making sure to dimensionally locate
it with respect to the datum axis.
3) Modify the locating dimensions to '0' in both the x and y directions.
4) #Pattern the feature.
5) Create a #Local Group of the datum axis and the pattern leader. This can
be achieved by selecting #Feature; #Group; #Local Group; #Range, and keying
in the feature number that pertains to the datum axis as the lowest member
of the #Range of features. After hitting #Return/#Enter on your keyboard,
enter the feature number that pertains to the leader of the pattern--and
then hit #Return/#Enter.
6) To pattern the pattern, choose #Feature; #Group; #Pattern, and select any
member of the #Local Group that you created. You will notice that the x and
y direction dimensions that you used to locate the datum axis will appear.
Use these dimensions as your 'driver' dimensions to pattern the pattern.
This way, you can always create a bi-directional, linear pattern of a
Pro/ENGINEER users can also radially pattern a radial pattern of features.
This can be
achieved by following the steps described below:
1) #Feature; #Copy; #Move; #Independent(The user must retain the
'Independent' setting); #Rotate on the existing radial pattern of features.
2) #Delete the entire original pattern--including its leader.
3) #Modify the 'copied' radial pattern's rotate copy angular dimension to
4) Create a #Local Group of the radial pattern of features.
5) Pattern the existing radial pattern by choosing the '0' angle dimension
as the 'driver'
dimension for a #Group; #Pattern.
In certain cases, the methodologies described above can dramatically reduce
model creation time with regards to feature duplication.
NOTE: The menu selections depicted above are for pre-Wildfire releases of
Pro/ENGINEER, but the same basic approach will work in Wildfire for
patterning a pattern.
Next post will be on how to create a table-driven pattern of a table-driven
I hope that some of you Pro/ENGINEER users can benefit from these patterning
Reply to
Loading thread data ...
Am I missing something? I can't seem to reference the axis (or datum point) created with offset info using Wildfire.
Reply to
In Wildfire the Sketcher will require you to go to the Sketch-References 'Select' pull-down menu and toggle to 'All Non-Dim. Refs' in order to be able to select a Datum Axis or Datum Point as a sketching Reference. You will notice that when you use a Datum Axis as the only Reference in your section sketch, the Pro/ENGINEER Wildfire Sketcher 'Intent Manager' will automatically locate(meaning dimension) your section sketch in both the X and Y directions with respect to the selected Datum Axis Reference.
Best of luck to you, and I hope that I helped you out with the difference in the way that Wildfire handles this situation.
Reply to

Site Timeline

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.