Outputting the location of a set of points at once

[AD_10323607]

I am making a spline in a part based on a large collection of points I am creating from a file.  When I assemble this part into an assembly I want to know the location of these points relative to the assembly coordinate system.  Is there a way for me to measure the x,y,z distance from the assembly coordinate system to those points all at once instead of having to do hundreds of individual measure commands?  Creo Parametric 8.0.5.0

[tbraxton · Accepted solution]

There is a quick workaround:

Import/Export

1) Create an IGES file containing only the point data of interest

      a) In the export dialogue ensure that only "Datum Curves and Points" is active

      b) Select a reference CSYS from your model used to generate the coordinates

      c) Save the IGES file

2) Modify this new IGES file extension by changing it from .igs to .pts file extension

3) Import this new .pts file into a new Creo model as follows

     a) Create a datum point feature using the offset csys option

     b) Select the reference Csys and import the .pts file from step 2, you will then see the table populated with the coordinate values

Refer to this thread which is relevant to what you are asking for other options. Solved: How to export a CSV file containing point coordina... - PTC Community

[AD_10323607]

Thanks for the quick workaround.  I was a bit worried when I saw that the IGES export had a lot more in it than just the points but this worked well.  Thanks!

[MD_9453627]

I have seen this solution in multiple searches but in Creo 8, I do not have an option to ensure that only "Datum Curves and Points" are exported.  It seems that export dialog box went away in Creo 4 (ref: https://community.ptc.com/t5/3D-Part-Assembly-Design/Creo-4-M010-issues-with-Assembly-and-IGES-output/td-p/116896).  I can't find any way to prevent exporting the part geometry which makes for some huge IGES files to sift through to find point data.  Is there an updated method that works with Creo 4+?

[kdirth]

The Save a Copy dialog changed in 4. Select Options to set export profile options. You now need to check the box, Customize Export, to get the window to pick export items.