Skip navigation
25695 Views 66 Replies Latest reply: Mar 26, 2014 12:52 PM by TomD.inPDX RSS
KevinBradberry Diamond 307 posts since
Jun 7, 2010
Currently Being Moderated

Apr 4, 2012 5:26 AM

Tips for text

Here's an open discussion for text and notes in Creo and Pro-engineer. 

 

Add tips and tricks that you know and ask questions that would be a good addition to this topic.

 

If you know of any previous threads that will compliment this topic please provide us the link.

    • John.Pryal Gold 305 posts since
      Jun 27, 2007
      Currently Being Moderated
      Aug 28, 2013 6:53 AM (in response to KevinBradberry)
      Re: Tips for text

      Here is one i strayed upon recently. If you have a multi line note with a leader, you can change the position of the leader line relative to the note itself, by adding @O to the start or end of a line. Apologies if someone already covered this, it is a rather long post.

       

      John

  • jonathan.hodgson Gold 413 posts since
    Nov 18, 2009
    Currently Being Moderated
    Apr 16, 2012 7:47 AM (in response to KevinBradberry)
    Re: Tips for text

    Multiple formats within single note

     

    To edit the style of one section of a note, first click to select the entire note, then click again to select just the section you want to change.  You can then RMB -> Text Style... and change size etc as required.

     

    This works directly with separate lines within a note, but to change just one part within a line you must first separate that section by adding {1: and } around the relevant text:

     

    {1:Large Text} Small Text

    Separate Line

     

    Then close the note editor and proceed as above.

  • SylvainA. Silver 245 posts since
    Jul 20, 2008
    Currently Being Moderated
    May 23, 2012 4:09 AM (in response to KevinBradberry)
    Re: Tips for text

    To insert text symbol directly from the keyboard (text symbol as a font): press CTRL+A when in a Note Properties window.

    To come back to standard font, press CTRL+B.

    In the exemple below I typed "azertyuiop"

     

    symbol.jpg

  • SylvainA. Silver 245 posts since
    Jul 20, 2008
    Currently Being Moderated
    May 23, 2012 4:29 AM (in response to KevinBradberry)
    Re: Tips for text

    To round the value of a parameter called in a note, add [.X] after the parameter name, X being the number of decimals.

     

    round.jpg

    • ptc-4888045 Copper 5 posts since
      Dec 18, 2012
      Currently Being Moderated
      Dec 18, 2012 10:57 AM (in response to SylvainA.)
      Re: Tips for text

      Hi I triedyour Tip, But It's not working in WF4

       

      I entered text notes as

       

      Volume Filled: &PRO_MP_VOLUME.X

       

      I am getting same as like text, If I remove .X then it's coming volume value without units and with 3 decimal places

  • SylvainA. Silver 245 posts since
    Jul 20, 2008
    Currently Being Moderated
    May 23, 2012 4:37 AM (in response to KevinBradberry)
    Re: Tips for text

    To see the result of a note change without closing the note window, simply click on your drawing's background when the changes are done.

     

    It will act like a "Preview" button.

  • ptc-4481803 Platinum 807 posts since
    Mar 5, 2012
    Currently Being Moderated
    Jul 9, 2012 6:24 AM (in response to KevinBradberry)
    Re: Tips for text

    What was the trick for putting in your own dimension?

    It has something to do with @D0 or something and then you type in your own dimension.

    • DomenicLaritz Silver 35 posts since
      Apr 22, 2009
      Currently Being Moderated
      Jul 9, 2012 6:36 AM (in response to ptc-4481803)
      Re: Tips for text

      @OmyOwnDimension - @O overwrites the default content

      • ptc-4481803 Platinum 807 posts since
        Mar 5, 2012
        Currently Being Moderated
        Jul 9, 2012 6:58 AM (in response to DomenicLaritz)
        Re: Tips for text

        Thanks. That is what I was looking for. Just remember it's an "O" (oh) and not a zero.

        • BrianMartin Diamond 1,212 posts since
          Feb 1, 2011
          Currently Being Moderated
          Jul 9, 2012 9:21 AM (in response to ptc-4481803)
          Re: Tips for text

          Hi Dale...

           

          In Wildfire 5 and beyond there's also a radio button for "Override" on the Dimension Properties window that does the same thing.

           

          Thanks!

          -Brian

          • ptc-1837901 Bronze 50 posts since
            Dec 21, 2007
            Currently Being Moderated
            Jul 10, 2012 1:02 AM (in response to BrianMartin)
            Re: Tips for text

            Just in case - remember it'll work only for reference dimensions created in drawing. You can't override value of model dimension, displayed in drawing with Show/Erase or Show Model Annotation.

            • BrianMartin Diamond 1,212 posts since
              Feb 1, 2011
              Currently Being Moderated
              Jul 10, 2012 11:47 AM (in response to ptc-1837901)
              Re: Tips for text

              t does work for dimensions created (and associative) in the drawing. I think what Lukasz was saying is that he's calling those "created" dimensions reference dimensions but in fact, this works for any created dimension.

               

              It does not work for "shown" or "driving dimensions" meaning the dimensions used to drive the 3D model. In most cases, though, this is not a big deal. Even for companies who insist upon "shown" dimensions, it's occasionally acceptable to create a dimension for special purposes like this.

              • ptc-1837901 Bronze 50 posts since
                Dec 21, 2007
                Currently Being Moderated
                Jul 10, 2012 12:44 PM (in response to BrianMartin)
                Re: Tips for text

                Yeah, that's right. I just called them "reference dimensions" since it's what they're called in Pro/E / Creo. But you're right, it's about all "hand-made" dimensions in drawing, as opposite to dimensions displayed or "showed" from the model. It was just a note in case someone start wandering why using @O option doesn't work or Override value box is not active.

  • TomD.inPDX Platinum 4,007 posts since
    May 25, 2012
    Currently Being Moderated
    Jul 9, 2012 10:54 AM (in response to KevinBradberry)
    Re: Tips for text

    If you don't want to mess with pen tables and you export PDF drawings, try assigning "thickness" to your text. 

    I use .012 in in/lb (SAE) drawings providing nice crisp text in the PDF export.

     

    Also, a nice font for distinguishing 1 (one) from I (upper case i) and l (lower case L) is ISO30985FONT.  It is the closest thing I found to the Creo Direct Modeling default HP font.

    • TomD.inPDX Platinum 4,007 posts since
      May 25, 2012
      Currently Being Moderated
      Jul 9, 2012 12:19 PM (in response to TomD.inPDX)
      Re: Tips for text

      Anyone know how to create the Feature Control Frame B below?

       

      http://www.kxcad.net/ugs/SDRC_I-DEAS_NX_series_Help_Library/des_ug/graphics/s8Dmgf2dobo.gif

      • BrianMartin Diamond 1,212 posts since
        Feb 1, 2011
        Currently Being Moderated
        Jul 9, 2012 12:32 PM (in response to TomD.inPDX)
        Re: Tips for text

        Hi Antonius...

         

        That's called a Composite Tolerance. from the Datum Refs tab, select the radio  button for Composite Tolerance. See below. If you need help with the other stuff (diameter symbols, etc) just let me know.

         

        composite.png

         

        Thanks!

        -Brian

        • TomD.inPDX Platinum 4,007 posts since
          May 25, 2012
          Currently Being Moderated
          Jul 9, 2012 3:19 PM (in response to BrianMartin)
          Re: Tips for text

          Sorry, I meant with the text editor.

          • BrianMartin Diamond 1,212 posts since
            Feb 1, 2011
            Currently Being Moderated
            Jul 10, 2012 11:28 AM (in response to TomD.inPDX)
            Re: Tips for text

            Hi Antonius...

             

            You can create everything but the initial large target using the text editor.

             

            I haven't tried playing with it. You may be able to come up with something close using text. If you're dead set against trying to use the GTOL features in Pro/E or Creo, your next best option would be to create a really nice custom symbol to do the job.  This might take a couple of hours to perfect, but I'm confident it can be done.

             

            This symbol could be made to satisfy all your needs. Actually, I can imagine quite a few people would like to get their hands on such a thing. Maybe you can take a crack at it. If you need help or get stuck, I'll be happy to help out. This might give people a "last resort" type of solution for times when they can't seem to get the internal GTOL functions working properly.

             

            Good luck... and if you decide you need help, just give a shout.

             

            Take care..

            -Brian

            • TomD.inPDX Platinum 4,007 posts since
              May 25, 2012
              Currently Being Moderated
              Jul 10, 2012 11:57 AM (in response to BrianMartin)
              Re: Tips for text

              Thanks again, Brian.  I appreciate both your observations regarding this functionality; re: in GTOL and the text limitation.

               

              I am certainly not against using GTOL as intended but it has to function in the drawings.  So far, I am getting nothing but flack from support in my request for getting the tagged datum planes to follow the hide/unhide properly.  That, and the system crashing when I move datum tags on the drawing are simply not workable.  Since I cannot reproduce the crash reliably, support will not do anything even with the crashlog in hand.  Remember that I also have a corrupt drawing file that will no longer allow me to move datum tags representing 2 days hard work.  So yes, I'd love to use GTOL... -IF- it worked correctly and reliably in drawings.

               

              The function of composite GTOL is relatively limited in my field.  I am sure I can find a way to "bury" the reference data well enough to create the rare occasion I need the composite GTOL within the model.

              • BrianMartin Diamond 1,212 posts since
                Feb 1, 2011
                Currently Being Moderated
                Jul 10, 2012 12:46 PM (in response to TomD.inPDX)
                Re: Tips for text

                I completely understand your frustration with the datum tag problem. This type of problem is the reason why many of the larger companies don't jump on the latest revision of the software. We hang back on purpose while the first few production releases are distributed. After 6-8 months, we finally start testing the "new" software. By that time, most of the larger, easy-to-catch bugs have been worked out.

                 

                As a side note... using TWO notes, I was able to duplicate the Composite Tolerance format. If you create a single note with the large datum target (at TWICE the text height as usual), you can then create a second note using the @[  and  @]  nomenclature to create text in a box.

                 

                The first note JUST has the large datum target in a box. The second has two lines using the @[ and  @] to create the necessary cells. Here's an image of the two notes side by side (click them for a better view, the lines come up faint until you click the images)...

                 

                tol1.png

                 

                And another of the two notes placed next to each other and grouped so they move together as one unit (again, click for a better view)...

                 

                tol2.png

                 

                The text for the two notes are as follows. All symbols are from the "Text Symbol" palette:

                 

                Note 1

                @[  <Datum Target Symbol> @]

                 

                Note 2

                @[  <Diameter Symbol> .004  <MMC Symbol> @]@[A@]@[B@]@[C@]

                @[  <Diameter Symbol>.002  <MMC Symbol> @]@[A@]

                 

                If you copy/paste those text notes and replace the symbols as noted, you can create a composite tolerance without using the GTOL system at all. Hopefully this gets you around the issue until PTC Customer Support can provide a resolution to your problem.

                 

                Take care...

                -Brian

                • TomD.inPDX Platinum 4,007 posts since
                  May 25, 2012
                  Currently Being Moderated
                  Jul 10, 2012 1:28 PM (in response to BrianMartin)
                  Re: Tips for text

                  I am really beginning to appreciate the power of the text editor in UG NX. 

                   

                  Happy to be on the front lines making your job easier at a later date, Brian

                  • TomD.inPDX Platinum 4,007 posts since
                    May 25, 2012
                    Currently Being Moderated
                    Jul 12, 2012 9:17 AM (in response to TomD.inPDX)
                    Re: Tips for text

                    Okay, I have another need...

                     

                    On the left is a valid datum tag and on the right is the best I can do with a note.

                     

                    Datum_tags_display.JPG  Also notice the difference in fonts.  I need the iso30985font with .012" thickness.  I cannot change the valid datum tag to match this customer requirement.

                     

                    Anyone have a trick in how to make the note look like the datum?

                     

                    BTW: crashed again this morning... I could be lighting cigars with $100 bills at this rate.

                    • BrianMartin Diamond 1,212 posts since
                      Feb 1, 2011
                      Currently Being Moderated
                      Jul 12, 2012 2:21 PM (in response to TomD.inPDX)
                      Re: Tips for text

                      Hi Antonius...

                       

                      As far as I can tell, that's the best I can do, too. I never knew you couldn't change the font for a datum tag. If you try to set the tag in the model, there's a Text Style button you can access... but it doesn't let you change font. it only allows you to change a few settings of the default font (and even those settings don't appear to work particularly well). If you try to set the tag in the drawing... you don't get the Text Style button at all! Either way, it doesn't much matter because you can't do anything with it.

                       

                      I got as sneaky as I could... I even changed the Default Text Font for the drawing without luck. I have to say, it's been awhile since I used any 3D annotations and I was fairly well shocked at how poor they work in Wildfire 5. I still need to go back and respond on the other thread about 3D annotation problems but I think these problems need to be pushed up to the Detailing Technical Committee ASAP so we can get them fixed.

                       

                      Thanks... and sorry I couldn't figure it out. I really hate when I get stumped!

                      -B

                      • BrianMartin Diamond 1,212 posts since
                        Feb 1, 2011
                        Currently Being Moderated
                        Jul 12, 2012 2:22 PM (in response to BrianMartin)
                        Re: Tips for text

                        Oh... and I meant to add the next best thing I can suggest is a custom symbol. That should get you around the problem.

                         

                        Thanks!

                        -Brian

                        • BrianMartin Diamond 1,212 posts since
                          Feb 1, 2011
                          Currently Being Moderated
                          Jul 12, 2012 2:57 PM (in response to BrianMartin)
                          Re: Tips for text

                          Egad... even the custom symbol idea is a harrowing nightmare. I was able to create a gorgeous symbol that does everything you want except for one very silly limitation. You cannot use a construction circle as the basis for a radial attachment point in a symbol. You also cannot use an arc (portion of a circle). It MUST be a full, solid circle... not a partial... not a construction.

                           

                          WHY?!  Geez do we really care if the symbol attachment point is based on the center of a construction circle (which does not show up on the field of the drawing)? Okay then so maybe I'll just use a teeny, tiny arc... solid... but so small it's not detectable. Nope. Doesn't work. What about a really big arc... 359 degrees? Nope. Doesn't work either.

                           

                          I've just joined the Detailing Technical Committee (took about a month to get on it). I can promise I will bring these issues up and see if I can get them resolved. These have to be very easy fixes.

                           

                          Thanks... and sorry this is such a pain!

                          • TomD.inPDX Platinum 4,007 posts since
                            May 25, 2012
                            Currently Being Moderated
                            Jul 12, 2012 3:58 PM (in response to BrianMartin)
                            Re: Tips for text

                            How do you get onto this committee?

                             

                            When I last used Pro/E for extensive detailing, we were still using the old style datum tags ( [-A-] ).  These were easy to fake in.

                             

                            In the drawing that caused the system to crash, I needed to tie the datum tag to a horizontal line representing a contiguous surface that the datum tag represents.  It simply couldn't be done since the line was a drafting sketch feature.

                             

                            I have a second problem with model generated datum tags in drawings.  The axial datum comes out bold (line thickness) while the tagged plane datum came out thin.  This is really a very lousy implementation.  Why am I the 1st to comment on this?

                            • BrianMartin Diamond 1,212 posts since
                              Feb 1, 2011
                              Currently Being Moderated
                              Jul 12, 2012 6:17 PM (in response to TomD.inPDX)
                              Re: Tips for text

                              You can sign up for the Technical Committees (abbreviated as just the "TC's") by going to ptcuser.org and clicking on PTC/User Technical Committees in the center of the homepage under "Get Involved". Here's a direct link to the Technical Committee homepage (Direct Link)

                               

                              Once you're on the homepage, click "Find a TC" from the left hand pane. If you're not yet a member of PTC/User, you'll have to sign up before you can go any further. Once you're signed up (totally free), you can see the various committees and select which one(s) you'd like to join.

                               

                              Participation in the TCs requires a bit of a commitment. Users are expected to participate in meetings and contribute to the group. Two face-to-face meetings occur each year- one in January at PTC Headquarters and a second one at the Planet PTC Live Event. Next years' Planet PTC Live event will be held in Anaheim (June 9-12). During these meetings, the entire committee has the opportunity to sit down with PTC developers and Product Line Managers. We discuss the software, enhancement requests, bugs, and ask questions to get answers "directly from the horse's mouth" so to speak.

                               

                              It took me quite a bit of effort to get onto the Detail TC (the committee concerned with drawing & detailing issues). Now that I'm on it, I'm anxious to start logging my feedback. I'm tempering this enthusiasm though because historically I know PTC hasn't put much into the drawing package. I also know this is intentional. As a long time user, I have felt (and continue to feel) that this is a critical mistake. If I had the ear of the developers, CEO, CFO, or anyone else who would listen, I'd try to steer them from this path. PTC has always believe that model-based engineering is the way forward and that paper is antique and archaic. While I agree, I can tell you from experience that most industries and most companies are not ready for this yet. It's just starting to get traction and adoption will continue to be painfully slow. In the meantime, people WANT and need drawing tools that work. In my opinion, PTC makes a tremendous blunder by allowing their competitors to service this space while they ignore it waiting for a day when their vision meets with reality.

                               

                              So... I joined the Detailing TC and I plan to do my best to push for enhancements. If not earth-splitting enhancements that create the drawing package we want, then at the very least fixing the bugs, closing the loopholes, and making the drawing package we already have work to it's optimum.

                              • TomD.inPDX Platinum 4,007 posts since
                                May 25, 2012
                                Currently Being Moderated
                                Jul 12, 2012 6:31 PM (in response to BrianMartin)
                                Re: Tips for text

                                Sweet, Brian.  I can think of no better voice in the committee than yours.  If it wasn't for the commitment for the face-time, I would be happy to participate.  I simply don't have funds to go flying all over the country on my dime.

                                 

                                If what you say is true, and if it continues, I will save my maintenance pennies and invest my $ and hours in SolidWorks or possibly Elements Direct.  At this point, I simply cannot make certified documents with the incomplete detailing tools in Creo/Pro.  This is certainly not acceptable on my end as this is how I make my living.  I will continue to submit support requests to achieve the minimal requirements to do my job.

                                 

                                Is it part of the committee's function to review SPR's submitted by users in relation to limitations and problems with making proper drawings?

                                 

                                I also submitted the recreation of the crash with datum tags in drawings.  very sad! 

                                Can I send PTC a bill for my lost hours to do what their QC failed to do?

                                 

                                Sorry Kevin, for hijacking your wonderful post.  I was hoping for answers, not more problems.

                                • BrianMartin Diamond 1,212 posts since
                                  Feb 1, 2011
                                  Currently Being Moderated
                                  Jul 12, 2012 7:05 PM (in response to TomD.inPDX)
                                  Re: Tips for text

                                  The TC's don't normally review SPRs as far as I know. But we do review enhancements and ideas submitted from committee members. I'd love to see the ideas from Planet PTC Community find their way to the TC's for voting, too. I've mentioned this to several people but I don't think we know what will "officially" become of the ideas from this site yet.

                                   

                                  There was a time I didn't hold out much hope to see meaningful improvements in the software owing to a sort of "tone deafness" from PTC. And, it's certainly fair to say maybe I am the only one who perceived that tone deafness. However, in the last couple of years I've seen real improvements in the way PTC has addressed some long-standing problems. For awhile I was cautiously optimistic. The first signs of progress were almost like seeing a mirage. I wasn't sure if I was really seeing what I thought I was seeing. But over the past 1-2 years I have to say, there's definitely something positive going on. Now, there are still problems... but it feels like PTC is really starting to listen. It feels like they're really starting to try to hear voices from the user community. This is real progress. They may have gone through the motions of listening and responding to criticism before... but now it feels like their heart is in it.

                                   

                                  I think that makes all the difference in the world. So now, I do have hope that we can improve the drawing package. I'll do whatever I can to pursue that goal. I'd encourage anyone else who'd like to join to visit ptcuser.org and learn more about the TC's.

                                   

                                  Take care...

                                  • TomD.inPDX Platinum 4,007 posts since
                                    May 25, 2012
                                    Currently Being Moderated
                                    Jul 12, 2012 7:38 PM (in response to BrianMartin)
                                    Re: Tips for text

                                    Yes, I'd seen this before in days long past but it was only a fizzle in the pan.

                                     

                                    Back on subject;

                                     

                                    YOU TOO CAN CREATE YOUR OWN FONT!  ( maybe I should define a "DATUM" symbol font set )

                                     

                                    Technically, the .fnt fonts, as compared to true type fonts, are simple micro-plotter files.

                                    They have a small definable grid in which you can define "move to" and "draw" commands between grid points.

                                     

                                    There are source files, index files, and compiled files.  Don't trust the source files, however since I have already decompiled a few fonts where the source and the decompiled versions did not match.  Another QC glitch!

                                     

                                    All the tools are there and the getting started manual has pretty much everything you need. 

                                     

                                    I do have one SPR into tech support.  The manual clearly states that the max text box height is 63, and there are fonts with heights up to 76.  Which one is in error?  That SPR has been submitted over a month ago and they assure me that they are still working on it.

                                  • ScottWyatt Copper 12 posts since
                                    Dec 16, 2009
                                    Currently Being Moderated
                                    Jun 25, 2013 8:21 AM (in response to BrianMartin)
                                    Re: Tips for text

                                    Brian Martin wrote:

                                     

                                    ...Now, there are still problems... but it feels like PTC is really starting to listen. It feels like they're really starting to try to hear voices from the user community...

                                     

                                    Do you still hold this opinion after the recent PTClive?  With respect to drawings in Creo?

  • TomD.inPDX Platinum 4,007 posts since
    May 25, 2012
    Currently Being Moderated
    Aug 1, 2012 1:01 PM (in response to KevinBradberry)
    Re: Tips for text

    I found this that might help this category:

     

    Use a $ in relations to use negative values -

     

     

    Relations


    All relations valid in a Creo Parametric model can be entered in a Pro/PROGRAM design.

    If an expression you want to include in the RELATIONS statement contains more than 80 characters, use a backslash (\) to interrupt the current line and continue the expression on the next line.

    The format can be as follows:

    RELATIONS  PARAMETER = COVER_SIZE/2 + LENGTH*0.75 -\  
    0.75*d3*d3 + THICKNESS*2  END RELATIONS

    Changing the material density in a part causes the system to update the mp_density value in relations and vice versa.

    Note

    • When using negative dimensions, a dollar sign ($) must precede the dimension symbol in both the input statement and the external input files. For example, use $d20 instead of d20. The dimensions will not be updated if a dollar sign does not precede the symbols. 
    • If the program assigns a value to a dimension variable that is already driven by a part or subassembly relation, two error messages appear. Edit or remove the program relation and regenerate.
  • TomD.inPDX Platinum 4,007 posts since
    May 25, 2012
    Currently Being Moderated
    Aug 1, 2012 1:32 PM (in response to KevinBradberry)
    Re: Tips for text

    Also found this:

     

    If you have a string of variables like in hole callouts, you noticed that you require spaces between the end of the variable and new text characters.  This is why you see...

    &THREAD_SERIES - &THREAD_CLASS

     

    UNF - 2B
    ...a text string which is obviously not to any standard that we as engineers accept.

     

    But there is a little known method to remove the requirement for the space:

    {0:&THREAD_SERIES}-{1:&THREAD_CLASS} ...which returns

    UNF-2B

    Old school editor but this is what makes it work.

     

    Why didn't PTC do this for the hole CALLOUT_FORMAT?

     

    PTC, are you listening?  This is what "we" call fit and finish

  • ptc-5156581 Copper 4 posts since
    Jun 21, 2013
    Currently Being Moderated
    Jun 21, 2013 7:23 AM (in response to KevinBradberry)
    Re: Tips for text

    Dear all,

     

    Sorry for push up the topic but i have a similar question on this subject.

    I try to find a way for create balloon in a text with using parametric like GD&T.

    I find nothing how to do that without use balloon and use related to object.


    Any idea ?

     

    Thanks

    • BrianMartin Diamond 1,212 posts since
      Feb 1, 2011
      Currently Being Moderated
      Jun 24, 2013 11:32 AM (in response to ptc-5156581)
      Re: Tips for text

      Hi Sebastien...

       

      Can you draw us a simple image of what you're trying to to. I'm not quite sure from your initial message.

       

      Thanks...

      -Brian

      • ptc-5156581 Copper 4 posts since
        Jun 21, 2013
        Currently Being Moderated
        Jun 25, 2013 8:00 AM (in response to BrianMartin)
        Re: Tips for text

        Hi Brian,

         

        I want to get something like that.

        Capture.PNG

         

        Balloon inside a note !

         

        Seb

        • ScottWyatt Copper 12 posts since
          Dec 16, 2009
          Currently Being Moderated
          Jun 25, 2013 8:41 AM (in response to ptc-5156581)
          Re: Tips for text

          I do think you can insert a symbol using a parametric reference, but it has to be created individually, brought into session, and you would need a seperate symbol for each number.

           

          Do you want a balloon note with a free text string or do you want a parametric reference to the BOM?  I don't believe we can access the Pro/report parameters outside of the repeat region.  Once your BOM changes, the notes will be discrepant. 

           

          I would love to be able to have a note like "Find No. &rpt.index.1" or something to that effect.  That way we don't have to worry about our notes being wrong or out of order.  I realize fixing the index is a possible solution but lets be honest, why can't we access the BOM?  The information is there, they just wont let us use it.

        • TomD.inPDX Platinum 4,007 posts since
          May 25, 2012
          Currently Being Moderated
          Jun 25, 2013 10:21 AM (in response to ptc-5156581)
          Re: Tips for text

          PTC is seriously lacking in this regard.  Every other package offers symbolic inline "flagging" if you will. 

          Maybe the "new and improved" detailing package long touted for Creo 3 will address this.

  • JWayman Silver 123 posts since
    Oct 7, 2010
    Currently Being Moderated
    Jul 11, 2013 2:42 AM (in response to KevinBradberry)
    Re: Tips for text

    Hello,

    I made a note and saved it for future use. The note looked something like this:

     

    note.jpg

     

    All well and good. However, when I inserted a note from file and selected the note I had saved, this is what came in:

     

    note 2.jpg

    Spot the difference?

    The word 'NOTES' is no longer underlined. How can this be?

    Am I doing something wrong, or is this a bug?

     

    Whilst on the subject, I know how to split up notes using {1:xxxx}{2:yyyy}, etc. so different bits can be formatted differently. However, if I format one of the text segments as Centre Justified, they all change. Likewise if I make just one Left Justified. Is it not possible to have different justifications in a single note?

     

    Thanks,

     

     

    John

     

     

    WF4, M220

    • ptc-5008082 Bronze 85 posts since
      Mar 13, 2013
      Currently Being Moderated
      Jul 11, 2013 3:32 AM (in response to JWayman)
      Re: Tips for text

      No idea about the underline, it just falls off!

       

      For the justification though, if you look at  the text style box it is split into 'character' and 'note/dimension'

      Stuff in the character area can be applied to individual portions of the note, whereas stuff in the note/dimension area is applied to the whole note - or at least that is my understanding of it (doesn't help you)

      Justifications can be applied to individual cells in a table but not lines in a note

      • JWayman Silver 123 posts since
        Oct 7, 2010
        Currently Being Moderated
        Jul 11, 2013 3:59 AM (in response to ptc-5008082)
        Re: Tips for text

        Thanks, Charlotte,

        I think I twigged where the underline goes: It is saved as a .TXT file, which is associated with Notepad, and does not support formatting such as underline. I don't know whether using Wordpad might help. I'll have a play one day when I have time.

        As far as the Justification goes, shame. It would be good to be able to create notes with varying justification, although the comments above regarding Notepad would probably apply equally.

        Ah! Well, never mind...

         

        John

        • dgschaefer Gold 340 posts since
          May 4, 2006
          Currently Being Moderated
          Jul 11, 2013 6:25 AM (in response to JWayman)
          Re: Tips for text

          Notepad or Wordpad isn't going to make a difference, unless you are opening the *.txt file in one or the other, editing and saving it.  I assume you're creating the note in Creo and saving it out as a *.txt file and then reading it back in.

           

          The *.txt format is 'plain text', so no formatting capabilities at all.  You can open a *.txt file in Wordpad, or Word for that matter, and add all kids of formatting.  It'll get stripped away, however, when you save it as a *.txt.

           

          The only way that Creo could save the formatting is if it used some kind of text based formatting language like HTML markup or something like that.The curly brackets is something like that but all it does is break up different text blocks so different formatting can be applied, it doesn't appear to actually mean anything specific.

    • TomD.inPDX Platinum 4,007 posts since
      May 25, 2012
      Currently Being Moderated
      Jul 11, 2013 7:40 AM (in response to JWayman)
      Re: Tips for text

      That formatting seems to go into some other register in the part/assembly/drawing file.  Have you tried to do a copy/paste from within the session for both of your instances?  If that works out, you could have a generic note part, similar to symbols.  Maybe even a custom symbol library for notes is the answer.

  • ptc-5012710 Copper 3 posts since
    Nov 22, 2013
    Currently Being Moderated
    Mar 26, 2014 5:48 AM (in response to KevinBradberry)
    Re: Tips for text

    Creo2 drawing notes image:

    CREO2-image.JPG

    Notepad notes image:

    Notepad-image.JPG

    Hello Team,

     

    Am just trying to fix the alignment problem with in Annotation->Note

     

    Why two lines are not getting aligned in creo 2 like how in Notepad.

     

    Your ideas will be really helpful.

    • ptc-4481803 Platinum 807 posts since
      Mar 5, 2012
      Currently Being Moderated
      Mar 26, 2014 5:58 AM (in response to ptc-5012710)
      Re: Tips for text

      Naveen,

      Welcome to the forum. PTC is in the process of creating an editor where "What you see is what you get" per this product suggestion. I am not sure if this is available yet, or if it is going to be in Creo 3.0

       

      Thanks, Dale

       

      http://communities.ptc.com/ideas/2059#comment-7802

    • StephenWilliams2 Bronze 73 posts since
      Jun 7, 2010
      Currently Being Moderated
      Mar 26, 2014 6:09 AM (in response to ptc-5012710)
      Re: Tips for text

      Are you using a font other than the default CREO "FONT"? There are several true type fonts that adjust width based on the letter or symbol therefore you won't be able to line up that kind of text.

       

      The CREO default "FONT" is a fixed width letter so it will align.

       

      I believe this is the same with Microsoft word when using fonts that are variable width.

       

      Steve

      • ptc-5012710 Copper 3 posts since
        Nov 22, 2013
        Currently Being Moderated
        Mar 26, 2014 6:13 AM (in response to StephenWilliams2)
        Re: Tips for text

        CREO2-fontstyle.JPG

         

         

         

        Hello

        Dale thanks for the update.

        Stephen thanks for your quick response, i am using default font for this text.

         

        Please suggest.

        • StephenWilliams2 Bronze 73 posts since
          Jun 7, 2010
          Currently Being Moderated
          Mar 26, 2014 6:33 AM (in response to ptc-5012710)
          Re: Tips for text

          Unfortunately "ISOFONT" is different from "FONT". It appears to me that your company default font is "ISOFONT". I double checked and "ISOFONT" is a variable width font meaning that the width of each character varies based on that character. So in your note, the "1. " is a different width than "   " (three consecutive spaces).

           

          You can verify this by changing from ISOFONT to FONT for this note and they should line up. Unfortunately if your company is strict about the font used, you may have issues with this internally. You can use this example to help them understand why they may want to consider the default font.

           

          I know that many companies don't like the "FONT" because of 1 (one) and I (capital letter i) are exactly the same.

           

          The default font can be changed in the drawing setup file. (FILE, PREPARE, DRAWING PROPERTIES, detail options (change), and look for the "DEFAULT FONT" OPTION.

           

          Steve

          • ptc-5012710 Copper 3 posts since
            Nov 22, 2013
            Currently Being Moderated
            Mar 26, 2014 9:43 AM (in response to StephenWilliams2)
            Re: Tips for text

            Hello Steve,

             

            I completely agree with you and tried the same. I couldn't convince for other fonts rather i am planning to use as is

            Thanks allot for your timely help(your points gave me a convincing reason to say its not possible )

             

            Naveen

            • TomD.inPDX Platinum 4,007 posts since
              May 25, 2012
              Currently Being Moderated
              Mar 26, 2014 12:52 PM (in response to ptc-5012710)
              Re: Tips for text

              I have jumped through the hoops of making special little text features to make it appear aligned.  Things like a space in superscript is about a half space and so forth.  There has to be a better way.

               

              I hope Dale is right that this is addressed in Creo 3.0.

               

              Unfortunately you cannot blank the outline of a table.  If you could, you can make your notes using a 2xn table to format your notes.

More Like This

  • Retrieving data ...

Bookmarked By (7)