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2582 Views 14 Replies Latest reply: Feb 22, 2012 7:07 AM by KevinBradberry RSS
ptc-4339982 Bronze 27 posts since
Nov 22, 2011
Currently Being Moderated

Feb 20, 2012 8:48 AM

Change dimension preferences

Hi I would like to know how to change the dimensions style in a drawing.

 

By standard the text is always viewed from below however I would like to have the vertical dimensions viewed from the right? I would also like all the text to sit above the dimension line.

 

I presume these are all editable somehow in the config file as is the case for most things in Creo. Is there a list of some sort which I can find which config options perform which changes?

 

Thanks in advance.

  • KevinBradberry Diamond 307 posts since
    Jun 7, 2010
    Currently Being Moderated
    Feb 20, 2012 11:28 AM (in response to ptc-4339982)
    Re: Change dimension preferences

    Hey Steve,

     

    You'll need to set the drawing option "text_orientation" to "parallel".  This is not a config option.  With an open drawing go to File>Drawing options.

     

    With drawing options, all options can be viewed on the list unlike config options in which you have to know the name of the option or use the search field to find it.

     

    If you want a serachable list for drawing options and config option, go to http://www.proesite.com/.  Click Utilities in the left margin and then click "check out my on-line utilities".

     

    -Kevin

      • KshetrabasiMahanta Gold 277 posts since
        Jul 31, 2011
        Currently Being Moderated
        Feb 21, 2012 4:26 AM (in response to ptc-4339982)
        Re: Change dimension preferences

        Hi Steve

         

        Drawing options can be saved as a .dtl file

        You can give the path of this (.dtl) file in your Config.pro in the following option

        drawing_setup_file      <Path of the file>

         

        Regards

        K.Mahanta

          • KevinBradberry Diamond 307 posts since
            Jun 7, 2010
            Currently Being Moderated
            Feb 21, 2012 6:42 AM (in response to ptc-4339982)
            Re: Change dimension preferences
            1. I don't have access to Creo 1.0, but in previous versions all drawing options can be viewed by scrolling when the drawing options dialog box is open.  File>Drawing Options.  Maybe the location has changed.  Type drawing options into the search field that Creo 1.0 provides for searching for commands (located about top right of window).
            2. I'm not sure what the second quesiton is asking, please clarify.  If you want a note for a hole, first it must be a created with the hole feature.  When annotating the drawing, use the Show Model Annotations command and use the tab with an A shown in the image, then click the view with the hole and select the hole note from the dialog box to apply it to the drawing.  To make changes to the note, select it, right-click, choose edit value and delete any parameters that you don't want.

            hole-note.PNG

               3.  The number of instances of patterend holes will be a part of the note when created as shown above.  Notice the (1) HOLE at the end of the note, this            means there is only 1 hole.  When patterend, it will change.

             

            Let us know of anythign else you need to know.

             

            -Kevin

              • KevinBradberry Diamond 307 posts since
                Jun 7, 2010
                Currently Being Moderated
                Feb 21, 2012 7:11 AM (in response to ptc-4339982)
                Re: Change dimension preferences

                For showing the number of patterned instances, see item 3 in my previous reply.

                 

                I cannot think of why you would not be able to select a centerline.  I've never had to change the config file to allow the selection of centerlines.  Is it that you cannot select a centerline when placing dimensions or is it that you cannot select them at any time?

                  • KevinBradberry Diamond 307 posts since
                    Jun 7, 2010
                    Currently Being Moderated
                    Feb 21, 2012 8:42 AM (in response to ptc-4339982)
                    Re: Change dimension preferences

                    Is your dimension attachment type set to entity?  If it is then, for now, I cannot think what is causing the problem.

                     

                    I would try recreating the centerlines if they were created in an older version of Pro/E. 

                     

                    In case its needed, see this thread for making centerlines: http://communities.ptc.com/message/176624#176624

                        • KevinBradberry Diamond 307 posts since
                          Jun 7, 2010
                          Currently Being Moderated
                          Feb 22, 2012 6:51 AM (in response to ptc-4339982)
                          Re: Change dimension preferences

                          I don't know how you used that &p17 function you mentioned, it did not work for me.

                           

                          I don't thik it will be necessary, though.  As we discussed earlier, the automatic hole note gives you the number of holes in the note.  It will give you the number of holes if you create an axis pattern or a 2 dimension pattern.  Then the note can be modified to match you drafting prefernces.

                           

                          This is the default note.  Notice the - ( 6 ) at the end.  I created a pattern that has 3 holes in one direction and 2 holes in the other.

                          HOLE_PATTERN_1.png

                          I modified the - ( 6 ) to show X6.  You could move it the beginning of the note as 6X if needed.

                          HOLE_PATTERN_2.png

                          Reminder: to edit the note, select it, right-click, pick edit value

                            • KevinBradberry Diamond 307 posts since
                              Jun 7, 2010
                              Currently Being Moderated
                              Feb 22, 2012 7:07 AM (in response to ptc-4339982)
                              Re: Change dimension preferences

                              There is something different about the methods that we are using.

                               

                              I changed the hole type to exclude the tapping (circled in red).

                              hole_pattern_4.PNG

                               

                              The note updated as expected.  The tap portion of the note was removed.

                              hole_pattern_3.png

                              Then, I deleted the note to see if Show Model Annotations would bring it back and it did.

                              Read the thread again and see if something doesn't make sense.

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