Skip to main content
N
npeters1-Visitor
1-Visitor
April 19, 2017
Question

Cannot figure out why when we plot our drawings our symbols show up below the text or at the bottom of the dimensions? Help...

  • April 19, 2017
  • 4 replies
  • 9578 views

Our symbols that we add to dimensions, such as diameter and the degree symbols, show up fine when we are editing our drawings, but when we go to plot they end up showing up at the bottom of the text?... not sure what the fix is, must be something in the config that i am missing? Thanks in advance!

4 replies

S
23-Emerald III
StephenW23-Emerald III
23-Emerald III
April 19, 2017

What font are you using?

N
npeters1-VisitorAuthor
1-Visitor
April 19, 2017

I thought it was just the standard symbol font? What config controls it?

S
23-Emerald III
StephenW23-Emerald III
23-Emerald III
April 19, 2017

In the drawing setup (not config), default_font option controls it. FONT is the Creo standard up to Creo 3.

If you are using a different font, it might be causing issues.

Can you include a typical screenshot of the problem?

    slapha
    slapha15-Moonstone
    15-Moonstone
    April 19, 2017

    May be related, We had an issue with our plotter where someone had shrunk the quantity value in a Reference balloon so the value was basically hidden under the REF. When someone went to plot it from a PDF to the Plotter the plotter increased the size of the font on that quantity. Other than getting rid of that tiny quantity value from the balloon I have yet to find a good solution. We rarely print on the plotter so it hasn't been a huge issue.

    My guess is some form of font conversion between the PDF and the Plotter. Like it's converting the TrueType font to some TrueType font (and size)it recognizes.

    Creo 4.0 did change the symbol palette fonts to use Arial WGL text fonts to support ASME and ISONORM LT to support ISO symbols. So while your text is "font" the diameter and degree symbol is probably using Arial WGL.

    For some of the symbols you could use the ALT-Key commands to get them in as font, but it doesn't have all the symbols. If you can't change the printer settings for interpreting TrueType fonts, I'd suggest trying stroke all fonts on the print settings in Creo.

    2017-04-19_11-33-08.png

    N
    npeters1-VisitorAuthor
    1-Visitor
    April 19, 2017

    All,

         Thank you for your responses/input, what we have come to figure out was that it was a setting in the active drawing options. The default for Creo 4.0 was set as

    symbol_font, and the setting was ASME, we altered it in our drawing.dtl file to LEGACY, and it has solved the issue.

    Thank you again for your input.

      M
      mender12-Amethyst
      12-Amethyst
      April 20, 2017

      This sounds like an issue (6355386) that was fixed in Creo 4 M020.  When you get that build or later, please check that you can use the new ASME symbol_font and the export works correctly.

      S
      SYNDAKIT15-Moonstone
      15-Moonstone
      November 10, 2017

      I am on Creo 4.0 M030 and this is still an issue. 

      J
      jim110-Marble
      10-Marble
      June 1, 2018

      We see the same thing. The fix was to change the value for symbol_font from asme to legacy (or stroke all fonts). Appears to be a bug with the ISO symbol enhancement in Creo 4.

      Terms & ConditionsAccessibility statement